Because the reader is dependent upon the ABAQUS libraries, this reader is only available for platforms supported by ABAQUS.

The reader is available in the following directory:

$CEI\ensight251\machines\win64\lib_readers\udr_abaqus

The ABAQUS ODB reader is the recommended method of importing ABAQUS data into EnSight.

Simple Interface Data Load

Load your geometry/results file (typically named with a suffix .odb) using the Simple Interface method.

Advanced Interface Data Load

Load your geometry/result files (typically named with a suffix .odb) using the Advanced Interface method.

Data Tab
Format	Use the ABAQUS_ODB format.
Set geometry	Select the geometry file (typically .odb) and click this button
Set results	Not used
Format Options Tab
Set measured	Select the measured file and click this button.
Reader GUI	User controls as shown below are available:
Load Surface Sets	Toggle ON (default) to load all Surface Sets
Load Node Sets	Toggle ON to load all Node Sets (default OFF).
Load "*All*" Parts	Often, ABAQUS parts that are simply the global element matrix are redundant (for example, E_ALL contains all elements). Toggle OFF (default) to skip loading Parts with all in their name, saving memory and time.
Load Freq Step	Often, ABAQUS will include multiple steps in an .odb file and the one desired is the modal analysis. Toggle this ON to skip all other steps loading only the frequency step (Default is OFF). If multiple frequencies, then each EnSight timestep now becomes a different frequency.
Load Element Faces	Toggle ON to convert Surface Sets with 3D elements with Face Sets into 2D elements using face specifications where indicated by the ABAQUS dataset. (default ON).
Load internal decomposition parts	Toggle ON to load internal decomposition sets (that show the parallel decomposition of the ABAQUS solver) as EnSight parts.(default OFF).
Load Analytical Rigid Surface parts	Toggle ON to load rigid surface parts as transient, rigid line segments that can be extruded in 3 dimensions. This can be done using a python script. Contact <support@ansys.com> for details. (default OFF).
Load History Data	Toggle ON to load History data which will load either as constants or as queries over time (default ON). Some datasets contain history data at extremely high sample rates with large number of xy data pairs. EnSight is not structured to be able to handle large numbers of queries with a large number of data pairs, and will abort the loading of history data if it encounters a data pair with more than 3000 samples. The reader will output a warning that it has aborted the history data read and that you can override this number; set the environmental variable on the server as follows: set ENSIGHT_READER_MAX_QUERY_PAIRS to the maximum number of pairs that you wish to allow and restart EnSight.
Interpolate History to Constants	History data is typically input to EnSight as queries (curves). EnSight has the ability to use constant (single values at each timestep) in ways that are not available to queries. If this is ON then History variables will be interpolated as EnSight Constants (if extrapolation is not necessary). If OFF then History variables will be read in as constants only if there is an exact one to one match of time values for each EnSight timestep (Default OFF).
Skip Last Frame if Suspect	If the ABAQUS solver crashes, it can dump out a variety of variable values for the last FRAME in the ODB file that may be spurious. Toggle this ON (default) to check the last FRAME in a STEP for an increase in the number of variables and, if so, skip it. Toggle this OFF to ignore warning signs and load the data from the last frame. If suspect values are found in the last FRAME, then NAN checking of each variable value is turned on, with NANs returned as zero (Default ON).
Smart Uniform Delta Time	Some ABAQUS STEPs have frame values that are constant (and very small). Frame values are used by EnSight for time steps and therefore from this type of STEP are not monotonically increasing in time and EnSight will skip these timesteps. Toggle this ON, and EnSight will automatically convert time values from selected ABAQUS STEPs into using a delta time of 1.0 (default is ON). Because EnSight is automatically changing the timestep values, this will only be done to selected ABAQUS STEPs (more may be added over time). The current list of these includes only one ABAQUS STEP: *STEP PERTURBATION, *STATIC. As new STEPs are encountered they may be added to this list and documented. If a new STEP is encountered with non monotonically changing time values that should be added to this list, please contact <support@ansys.com> and send us an example dataset. And the workaround is to toggle ON the other toggle Uniform Delta Time which will make the delta time = 1.0 for ALL timesteps for all ABAQUS Frames in all ABAQUS STEPs. Because this changes the ODB time values, this Toggle was added to allow you to turn this off and use the frame values as the time values in EnSight.
Uniform Delta Time	Some ABAQUS STEPs have Frame values that are constant (and very small). Frame values are converted to float values and are used by EnSight for time steps. Time values may therefore become not monotonically increasing in time and then EnSight will skip these timesteps. Toggle this ON, and EnSight will automatically convert ALL ABAQUS Frame time values from all ABAQUS STEPs into using a uniform delta time of 1.0. Because this changes the ABAQUS ODB time values for ALL of the ABAQUS STEPs it is by default OFF.
NaN Check	The ABAQUS ODB solution data is converted in the ODB API from double precision EnSight single precision, float. The default is to check all floating point values and to print a warning in the message window if there is a problem. This conversion of the raw data sometimes results in Not A Number values or denormalized floats (almost NaNs which should not be used in further calculations). If you get a warning in the message box that you have denormalized floats, try checking the message window for Extrapolate Variables to Nodes (see below).
Extrapolate Variables to Nodes	Variable values are extrapolated to the nodes using the ABAQUS internal API from each element's internal integration points to the nodes from each element. The reader then does a simple average of the nodal values from each element. This has been demonstrated to give the same results as ABAQUS CAE. Because the simple averaging is done within the ABAQUS API, it has been seen to eliminate some of the NAN issues described above.
Load Warn parts	The ODB dataset includes subset parts that contain exist to Warn the user of element or variable anomalies. Often this can result in an excessive number of parts in the EnSight part list. Toggle ON to load parts starting with Warn* (default) and OFF to skip these parts. It is recommended that you skip these parts if EnSight is slow to load data or activate variables due to a large number of parts.
Use Section	Shell elements include variable data for each section. This reader allows the use of the First (default) or the Last section.
Integration Point	Shell elements include variable data for each of several integration points. Choose max, min or average (default).
Console Output	Normal - Informational and error output to the console. Verbose - Detailed informational and error output to the console. Debug - Step by step progress through the reader with detail numerical output for results to the console. None - No console output
Instance	Choose an instance (1 to the number of instances). Default is to load them all.
Step	Choose a step (1 to number of steps). Default is to load all non-frequency steps.
Shell Section	Which shell section to use (1 to number of shell sections).
Starting Part Number (1 to num)	Which part to begin loading (default is empty which is the first part).
Ending Part Number (1 to num)	Which part to end loading (default is empty, which is last part).

Older Version ODB Files

The EnSight ODB reader will be able to read .odb files from 6.1 to the current version using the upgrade utility. If upgrade is needed, the original ODB file is read in and left unchanged, while an upgraded copy is automatically written in the same directory (user must have write permission in this directory). UPGRADE_6_* is added to end of filename prefix, where the * is the current library version, for example UPGRADE_6_14 for ODB library version 6.14. The current library version can be seen in the file open dialog under the Data tab, when you choose the ABAQUS_ODB reader in the reader selection pulldown in advanced mode. The reader version will appear just below the pulldown in the reader description box.

The first numbers (for example, v2018) indicate the API (which corresponds to solver version 2018) as shown in the above figure.

Shell Elements

In ABAQUS, many shell elements have sections and integration points. Sections are regions such as top or bottom of a beam. Integration points are specified locations on the sections. In contrast, EnSight elements have only one value per element. So it is necessary to have a mapping scheme between the multiple element values in ABAQUS and the single EnSight elemental value. Choose the Format options tab in the data reader dialog to change the mapping of shell elemental variable data from ABAQUS to EnSight.

Integration Point pulldown allows the choice of the max, min or average (default) of the integration points at a shell element to use as the EnSight variable value.

The Use Section pulldown allows the choice of the first (default) or last section at a shell element to use as the EnSight variable value.

To enter in a section number of your choosing (if there are more than two), simply enter a value (1 to number of sections) into the Section field. Entering a value into this field (default is empty) supersedes the choice in the pulldown.

Modal Data

Sometimes the analysis will have transient/static STEPs along with FREQUENCY STEPS. EnSight can handle either transient/static or frequency data, so by default, with mixed data, the FREQUENCY STEPs are skipped, and only the transient/static STEPs are loaded.

If you want only the modal data, toggle ON the Load FREQ STEP toggle, and the reader will use the first modal frequency STEP. Also, if, for example, you know the modal FREQUENCY STEP, you can also select the step number by entering it in the STEP (1 to num) field

Once your modal data is loaded, to visualize the modal displacement, select the part(s) of interest, and displace by the displacement vector, U. Each modal frequency is loaded in as a separate EnSight timestep, so step through EnSight "times" to step through the frequencies. Similarly you can view the modal velocity, V or the acceleration, A.

Each modal frequency is stored as a single value for a given EnSight timestep. You can access these EnSight constants as follows:

Modal Frequencies (single value constants) are stored in the constant, single value variable, H_EIGFREQ. Modal Eigen values (single value constants) are stored in the single value variable H_EIGVAL.

Modal Participation Factors (single value constants) are as follows:

Analytical Rigid Surfaces

ABAQUS ODB data includes three Analytical Rigid Segments that do not have variable data, do not deform, and only move rigidly in translation or rotation that are of type

Analytical Rigid Surfaces Manual Creation

In order to turn the Analytical Rigid Segment into an Analytical Rigid Surface, you can use EnSight's Extrude function. If the segment part has REV in the name, then you'll want to rotate, and you can toggle ON to rotate about a part centroid, and choose the part id of the rigid reference node corresponding to this ARS part, pick the rotational degrees and the axis, and click Create to construct the extruded rotational surface.

Analytical Rigid Surfaces Automatic Creation Using Python Tool

Should you want all of this done for you automatically, there is a python tool included with EnSight that will automatically create all of your Analytical Rigid Surfaces. As shown in the figure below, simply click the tools icon at the top and choose the Create ARS icon under the Visualize folder. Simply fill in the graphical user interface and it will turn on computational displacements of the rigid reference nodes automatically and just create the rigid reference surfaces as expected.

Figure 2.2: Analytical Rigid Surface Python Tool

If the default behavior of the reader is unexpected (that is, no parts loaded, too few timesteps loaded, or variables not available) then reload the .odb file and select the Format options tab and choose Console Output: Debug. Then take a look at the output in your server console.

Missing Parts

Are you missing parts? By default, EnSight does not load the nodesets. Toggle this ON to load the nodal parts. By default, EnSight does not load parts whose names containing ALL or All because these are often duplicate parts that double the required memory and slow down the operation of the reader. Toggle ON the Load *all* toggle to load these parts. If you have no parts loaded, take a careful look at the console output (see below) and notice that all of the nodesets are skipped, as is the ALL_ELEMENTS part, therefore you have no parts loaded.

-----------------------------------------------------------
              EnSight ABAQUS Parts
              Total num Instances 1
              Total num nodes 936
              Total num elements 625
    Choose 'Format options' tab in data reader dialog
    To load or skip node or surface sets:
        Toggle OFF 'Load Surface Sets'
        Toggle OFF 'Load Node Sets'
    To load or skip sets with ALL in their name:
        Toggle OFF 'Load *ALL* Parts'
-----------------------------------------------------------------------------------
    ABQ Ens Part Instance & Type Number Status
    Num Num Name Elements
------- ------ --------------- --------- -------
1. 1. ALL NODES Assm 0 Nodeset 1 SKIPPED
2. 1. ALL NODES Assm 1 Nodeset 936 SKIPPED
3. 1. ASSEMBLY_CONSTRAINT-1_NODES Assm 1 Nodeset 36 SKIPPED
4. 1. ASSEMBLY_CONSTRAINT-1_POINT Assm 0 Nodeset 1 SKIPPED
5. 1. ALL ELEMENTS Assm 1 Elemset 625 SKIPPED
-----------------------------------------------------------
Number of regular ABAQUS parts = 5
Number of Analytical Rigid Surface parts = 0
Total number of Abaqus parts = 5
Total number of EnSight parts = 0
-----------------------------------------------------------
-----------------------------------------------------------

Missing Timesteps

Are you missing timesteps? Each ABAQUS FRAME is an EnSight timestep. If the change in time between two successive frames is too small to represent as a float value, then EnSight will skip it.

ABAQUS data is loaded in STEPs. Since EnSight has only timesteps (transient) or one timestep (static) there is a bit of mapping that goes on to read in an odb dataset.

ABAQUS STEPs of type *STEP PERTURBATION, *STATIC" STEP are now loaded with their timesteps incremented by 1.0. The Toggle Smart Uniform Delta Time has been added to turn this off and use the frame values (which are 2E-16). This is ON by default.

To pick a given ABAQUS STEP, for example, STEP 4 (1- based), simply enter 4 into the STEP (1 to num) field.

Here is the details on the load steps and times and is consistent with ABAQUS handling of .fil.

ABAQUS STEP is an EnSight Case. Each ABAQUS FRAME is a time increment to the final STEP value. The EnSight total time is a unique cumulative value for each EnSight timestep that is monotonically increasing.

Each odb STEP is like a sequential, but separate analysis.

The ODB API reports data by STEP with each step having a series of FRAMES each representing an EnSight timestep. EnSight use the ABAQUS TOTAL TIME as our Solution Time. Apparently, an ABAQUS user can look at their status file and know what TOTAL TIME relates to the STEP.

If we had a file with 3 ABAQUS STEPS, and 5 increments per step:

Notice the ABAQUS odb details in the left columns and the resulting EnSight mapping on the right. The X is a timestep that is excluded from EnSight because there is no time change from the previous step.

Therefore, if you wanted to look at:

The 1st load case (STEP 0): Look at Ensight times 0 - 0.3 or EnSight steps 0 - 2

The 2nd load case (STEP 1): Look at Ensight times 0.35 - 1.8 or EnSight steps 3 - 6

The 3rd load case (STEP 2): Look at Ensight times 1.8 - 7.8 or EnSight steps 6 - 9

---

Note:  Times that have no total time increment are dropped from EnSight.

---

Times that have an extremely small increment (for example, 1E-10) are incremented larger so that the time can be represented as a float.

For example, when you see the X in the left hand column below, this timestep is skipped because you can see that the increment is essentially zero. A number of steps are skipped below for that reason.

Missing Variables

When you choose Console Output Debug, you can see the list of variables in the console output and that some of the variables are skipped. Skipped variables include the _MAG variables, which are vector magnitude that EnSight auto-calculates for vector variables from the components. You can see that some of the contact variables, which are part-specific are combined into one, single value.

Odd Part Shapes

When you read in your parts if the Surface Set parts seem to have full elements showing and you only want the selected faces of the elements to be used to form your parts, then reload your data and choose Load Element Faces in the Format options tab of the Data Reader dialog.

Figure 2.3: Surface Set Part

See Read Data

The current Fluent Direct Reader also reads Ansys Airpak and Ansys Icepak data. The Fluent Direct reader typically loads a Fluent case (.cas) file and the matching data (.dat) file. However, Ansys Airpak and Ansys Icepak writes out a .fdat file which doesn't automatically get recognized by the EnSight Fluent reader and some extra understanding (and sometimes user-intervention) is necessary as described below.

See the following files for the latest information on the Fluent reader.

$CEI/ensight251/src/readers/fluent/README.txt

The comments that follow are for the current Fluent reader. The reader loads ASCII, binary single precision, or binary double precision. The files can be uncompressed or compressed using gzip.

Data File Description

Icepak can generate files: filename.cas, filename.dat just like Fluent, but also if the analysis uses a nonconformal mesh (not available in Fluent) then there will be filename.fdat, and filename.nc.cas files. The filename.nc.cas is a nonconformal mesh geometry and its matching results file is the filename.fdat file.

Simple Interface Data Load

Load your geometry file (typically named with a suffix .cas ) using the Simple Interface method. EnSight will automatically load the matching .dat file. However, if you want to load the filename.nc.cas data file and its corresponding filename.fdat file, then you will either need to rename it to match exactly and have the .dat extension (filename.nc.dat), or go to the advanced data load.

See Read Data and Fluent Direct Reader.

Description

This reader from AcuSim will read results from Acusolve. Select the .log file from the simple or advanced interface.

File → Open...

The File Selection dialog is used to specify which files you wish to read.

File → Open...

Simple Interface Data Load

Load your AcuSolve .log file using the Simple Interface method.

Advanced Interface Data Load

Load your AcuSolve .log file using the Advanced Interface method.

Data Tab
Format	Use the AcuSolve format.
Set file	This field contains the first file name. For the first file you should choose a file with extension .log. Clicking button inserts file name shown into the field. Loading the .log file will load all both geometry and results.
Format Options Tab
Set measured	Select the measured file and click this button.
Other Options
Reset time	When toggle is on, time begins at 0.0 (default is off).
Extended output	When toggle is on, console output will be verbose (default is off).
Mesh Motion	When toggle is on, moving meshes are visible (default is on).
Unique parts	When toggle is on, a unique set of surfaces is shown in the part list (default is off).
Additional runs	Enter the comma separated list of runs (3, 5, 10, 10:20:2), or _all. (default is _none).

Read Data

Three Ansys Readers

There are three Ansys readers available in EnSight: two older, unsupported legacy readers and the supported Ansys Results. Long-term, Ansys Results is the reader of choice. This reader should read the latest Ansys results as well as older versions. The other two, legacy readers will not show up in the reader list by default and will not be documented in this manual.

Legacy Reader Visibility Flag

The older readers, by default, are not loaded into the list of available readers, and are not discussed in the remainder of this document. In the unlikely event you need to enable these readers, go into the Menu, Edit → Preferences and click on Data and toggle on the reader visibility flag. The legacy reader documentation is found in $CEI/ensight251/src/readers/ansys/README and is not included here.

Ansys Results Reader

The Ansys Results reader supports scalar, vector and tensor variables, including the capability to compute several common scalar variables derived from tensors (such as the common failure theories) as well as local element result components (such as axial stress in truss elements) when such element results are available. Additionally, there is some control over the creation of variables from element-based results. For example, they can be averaged to the nodes (with or without geometry weighting) if desired. See the format options below for more details.

Results are always presented in the global coordinate system. Therefore, any results in local coordinate systems, or in non-cartesian coordinate systems are transformed as needed into the model system.

For shell elements that have multiple layers (sections), you can choose the section that will be used. Additionally, you can choose to have a different variable be created for each section. See format options below for more details.

You can control how parts are created. Parts can be created according to the part id, the property id, or the material id.

Ansys has added a new data compression algorithm (sparsification) to the output of Ansys Mechanical that has caused read failures in the EnSight Ansys mechanical reader when, for example attempting to open some .rst files. This reader now supports datasets utilizing this compression algorithm.

Simple Interface Data Load

Load your geometry/results file (typically named with a suffix .rst) using the Simple Interface method.

Advanced Interface Data Load

Load your geometry/result files (typically named with a suffix .rst) using the Advanced Interface method.

Data Tab
Format	Use the Ansys Results format.
Set file (or results)	Select the geometry/results file (typically .rst, .rth, or .rmg) and click this button
Format Options Tab
Set measured	Select the measured file and click this button.
Other Options
	Include any Element sets defined. These are sets of full elements which are generally some logical subset of the total number of elements. Default is on.
Include Face/Edge Parts	Include any Face or Edge sets defined. These are some logical set of particular faces and/or edges of full elements. Default is off.
Include NodeSet Parts	Include any Node sets defined. These are generally the subset of nodes needed for the Element, Face, or Edge sets above. As such, they are generally not needed as separate parts, but can be created if desired. Default is off.
Include local elem res comps (if any)	Include the local stresses components, etc that are in the element's local system. A simple example is a bar (such as a truss element), which only has tension or compression in the element's axial orientation. Such an element would have an axial stress variable. Other elements would have appropriate result component variables. Default is on
Include Tensor derived (VonMises, etc.)	For tensor results, calculate scalars from the following derived results (principal stress/strains, and common failure theories): Mean Equal Direct VonMises Min Principal Octahedral Mid Principal Intensity Max Principal Max Shear By default, all 9 of these will be derived. You can control which are created by this toggle, with an environment variable. Namely, setenv ENSIGHT_VKI_DERIVED_FROM_TENSOR_FLAG n where n = 1 for Mean only 2 for VonMises only 4 for Octahedral only 8 for Intensity only 16 for Max Shear only 32 for Equal Direct only 64 for Min Principal only 128 for Mid Principal only 256 for Max Principal only 512 for all or any legal combination. example: for VonMises and Max Shear only, use 18. Default is on.
Force Static Zero Timevalue	Make the RST file return single time step for static data and apply Displacements by default.
Regular Part Creation Convention	Parts will be created according to the following: Use Part Id - Part Id (this is the default) Use Property Id - Property Id Use Material Id - Material Id
Var naming convention	Use Content Field (if provided) - Variable names will be what is in the Content field, if provided. If not provided, they will be the VKI dataset name. This is the default. Use VKI dataset name Variable names will be the VKI variable dataset name (which are reasonably descriptive).
Element Vars as	Single element values - Element results (whether centroidal or element nodal) will be presented as a single value per element. Therefore will be per_elem variables in EnSight. This is the default. Averaged to node values - Element results (whether centroidal or element nodal) will be averaged to the nodes without using geometry weighting. Therefore will be per_node variables in EnSight. This is a global averaging, so shared nodes are affected by all parts that share a node. Geom weighted average to node values - Element results (whether centroidal or element nodal) will be averaged to the nodes using geometry weighting. Therefore will be per_node variables in EnSight. This is a global averaging, so shared nodes are affected by all parts that share a node. Ave to node values <by parts> - Element results (whether centroidal or element nodal) will be averaged to the nodes without using geometry weighting. Therefore will be per_node variables in EnSight. This is a local averaging, so all averaging is contained within each part. Geom weighted ave to node <by parts> - Element results (whether centroidal or element nodal) will be averaged to the nodes using geometry weighting. Therefore will be per_node variables in EnSight. This is a local averaging, so all averaging is contained within each part.
Post Midside Node Averaging	Average per_elem or per_elemnode data to nodes in models Off - No midside node averaging. For per_elem vars only (default) - Midside node averaging of element results only. For per_elemnode only - Midside node averaging of element node results only. These variables will have _el appended to the name. Both - Both per_elem and per_elemnode are considered.
If Sections, which:	Which section will be used to create the variable First - The first section will be used (this is the default) Last - The last section will be used Section Num (below) - The section number entered in the field below will be used Separate Vars per Section - A separate variable will be created for each section.
If Section Num, 1-based integer value:	If the previous option is chosen to be Section Num, then the value in this field is the 1-based section number to use to create the variable.

Limitations

EnSight is designed to post process results independent of any solver. As such EnSight lacks tools and tight integration with the Ansys Mechanical solver that are necessary for some Mechanical Analyses such as the following:

Data files from these analyses may read fine into EnSight but they will be lacking the necessary variables and/or the tools required for accurate, timely post-processing of these analyses.

Read Data.

Ansys Common Fluids Format (CFF) Post, is intended to be a post processing format whose variable values are the same as those shown in the native solver post processor. In EnSight, the Ansys Fluids Post reader was written to read Ansys Common Fluids Format files written 2020 R2 onwards, which includes the following: (the project file (.flprj) which will load the .cas.post and .dat.post files) by Fluent, (the project file (.flprj) which will load the .cas.cff and .dat.cff files) by CFX, (.cas.fsp and .dat.fsp) by FENSAP and (.cas.poly and .dat.poly) by Polyflow Classic. This reader uses the Ansys CFF SDK (R25.1) to read all of the information from the .cas.(post/cff/fsp/poly) and .dat.(post/cff/fsp/poly) files. This reader relies entirely on CFF SDK to provide necessary information to create parts and variables. The Project file is required to determine the correct time value for transient solutions. In addition, project file contains flags which are used by reader to determine about changing connectivity and coordinates (and is therefore strongly suggested for transient runs) if it is available (FENSAP and Polyflow Classic do not yet export the project file).

Simple Interface Data

Load Fluent exported .cas.post and .dat.post files using the project file (.flprj) if it is available. You should provide the project file(.flprj) if it is available, otherwise .cas.post file, and EnSight will attempt to read similarly named .dat.post files as well. EnSight will similarly attempt to load CFX exported (.cas/.dat).cff (via the project file), FENSAP exported (.cas/.dat).fsp or Polyflow Classic (.cas/.dat).poly files.

Advanced Interface Data

Load Fluent geometry and result information (typically named with suffix .cas.(post/cff/fsp/poly) and .dat.(post/cff/fsp/poly) respectively) which has been exported from Fluent/CFX/FENSAP/Polyflow Classic 2020R2 or later.

.cas.post

If the project file (.flprj) is available, select and click Load All Parts, otherwise if the project file is unavailable, select the geometry file (typically .cas.(post/cff/fsp/poly) and click this button. For transient geometry data, if the project file is unavailable, use a single asterisk to replace the step or time number (*.cas.(post/cff/fsp/poly).

.dat.post

Select the results file (typically .dat.(post/cff/fsp/poly) and click this button. For transient variable data, use a single asterisk to replace the step or time number (*.dat.(post/cff/fsp/poly). There is no need to select result file(s) if project file is provided as mentioned above.

Table 2.1:

Data Tab
Format	To use the reader, choose Ansys Fluids Post format.
.cas.post	Select the geometry file (typically .cas.(post/cff/fsp) and click this button. For transient geometry data, use a single asterisk to replace the step or time number (*.cas.(post/cff/fsp). If project file (.flprj) is available, select and click on Load All Parts
.dat.post	Select the results file (typically .dat.(post/cff/fsp) and click this button. For transient variable data, use a single asterisk to replace the step or time number (*.dat.(post/cff/fsp). There is no need to select result file(s) if project file is provided as mentioned above.
Format Options tab
Other Options
Console Output	Normal/Verbose/Debug adjusts the output information to assist in debugging issues.
Maximum number coprocessing timesteps (default 0, off)	This allows EnSight to post process a running, transient solution (e.g. coprocess), checking for new cas.(post/cff/fsp) and dat.(post/cff/fsp) (1 per timestep) as the solution proceeds and adding timesteps to the time dialog as they are encountered. If non-zero, this specifies the maximum number of possible timesteps that will be written out during this solution. This is useful to monitor a running solution or to begin post processing a long run without waiting for it to finish.

Caveats

Description

Reads a series of .adres files as a transient solution. Simply select one of the .adres files and the sequence will be detected. Requires that the .adres_base files exists in the same directory. Supported only on Windows.

File → Open...

The File Selection dialog is used to specify which files you wish to read.

File → Open...

Simple Interface Data Load

Load your Autodyn .adres file using the Simple Interface method.

Advanced Interface Data Load

Load your Autodyn .adres file using the Advanced Interface method.

Data Tab
Format	Use the Autodyn format.
Set file	This field contains the first file name. For the first file you should choose a file with extension .adres. Clicking button inserts file name shown into the field. Loading any .adres file will load all .adres files in the directory which includes both geometry and results.
Format Options Tab
Set measured	Select the measured file and click this button.
Other Options
	Include any Element sets defined. These are sets of full elements which are generally some logical subset of the total number of elements. Default is on.
Include Face/Edge Parts	Include any Face or Edge sets defined. These are some logical set of particular faces and/or edges of full elements. Default is off.
Include NodeSet Parts	Include any Node sets defined. These are generally the subset of nodes needed for the Element, Face, or Edge sets above. As such, they are generally not needed as separate parts, but can be created if desired. Default is off.
Include local elem res comps (if any)	Include the local stresses components, etc that are in the element's local system. A simple example is a bar (such as a truss element), which only has tension or compression in the element's axial orientation. Such an element would have an axial stress variable. Other elements would have appropriate result component variables. Default is on.
Include Tensor derived (VonMises, etc.)	For tensor results, calculate scalars from the following derived results (principal stress/strains, and common failure theories): Mean Equal Direct VonMises Min Principal Octahedral Mid Principal Intensity Max Principal Max Shear By default, all 9 of these will be derived. You can control which are created by this toggle, with an environment variable. Namely, setenv ENSIGHT_VKI_DERIVED_FROM_TENSOR_FLAG n where n = 1 for Mean only 2 for VonMises only 4 for Octahedral only 8 for Intensity only 16 for Max Shear only 32 for Equal Direct only 64 for Min Principal only 128 for Mid Principal only 256 for Max Principal only 512 for all or any legal combination. example: for VonMises and Max Shear only, use 18. Default is off.
Regular Part Creation Convention	Parts will be created according to the following: Use Part Id - Part Id (this is the default) Use Property Id - Property Id Use Material Id - Material Id
Var naming convention	Use Content Field (if provided) - Variable names will be what is in the Content field, if provided. If not provided, they will be the VKI dataset name. This is the default. Use VKI dataset name Variable names will be the VKI variable dataset name (which are reasonably descriptive).
Element Vars as	Single element values - Element results (whether centroidal or element nodal) will be presented as a single value per element. Therefore will be per_elem variables in EnSight. This is the default. Averaged to node values - Element results (whether centroidal or element nodal) will be averaged to the nodes without using geometry weighting. Therefore will be per_node variables in EnSight. This is a global averaging, so shared nodes are affected by all parts that share a node. Geom weighted average to node values - Element results (whether centroidal or element nodal) will be averaged to the nodes using geometry weighting. Therefore will be per_node variables in EnSight. This is a global averaging, so shared nodes are affected by all parts that share a node. Ave to node values <by parts> - Element results (whether centroidal or element nodal) will be averaged to the nodes without using geometry weighting. Therefore will be per_node variables in EnSight. This is a local averaging, so all averaging is contained within each part. Geom weighted ave to node <by parts> - Element results (whether centroidal or element nodal) will be averaged to the nodes using geometry weighting. Therefore will be per_node variables in EnSight. This is a local averaging, so all averaging is contained within each part.
If Sections, which:	Which section will be used to create the variable First - The first section will be used (this is the default) Last - The last section will be used Section Num (below) - The section number entered in the field below will be used Separate Vars per Section - A separate variable will be created for each section.
If Section Num, 1-based integer value:	If the previous option is chosen to be Section Num, then the value in this field is the 1-based section number to use to create the variable.

See Read Data.

The AVUS reader has been recently renamed, and was formerly called the COBALT reader.

There are two distinct readers for AVUS data (formerly Cobalt60) -- one for static data, AVUS (formerly Cobalt60), and one for transient solution data, AVUS Case (formerly Cobalt60 Case).

Both readers will read formatted and unformatted (single or double precision) Cobalt60 grids, solution files (pix files), and Cobalt60 restart files. The file format is determined automatically by the reader. The readers also support an enhanced solution (pix) format that contains additional solution data beyond the normal six fields.

See the following README file for current information on this reader and contact the author as listed in the README file for further information.

$CEI/ensight251/src/readers/avus_cobalt_2/README

Simple Interface Data Load

Load your geometry file (typically named with a suffix .grd) using the Simple Interface method.

Advanced Interface Data Load

Load your geometry and restart files (typically named with a suffix .grd and .pix) using the Advanced Interface method.

Example CSC File

Suppose you have the following files in the subdirectory.

/scratch/data/ensight/avus/mach6
file0200.pix  file0600.pix  file1000.pix  mach6_5.grd       mach6_path.csc
file0400.pix  file0800.pix  mach6_5.bc    mach6_nopath.csc  mach6_winpath.csc

Then your case file, mach6_path.csc, which includes the paths, will contain the following 4 lines as follows, where the 3rd line tells the reader that there will be multiple .pix files and the fourth line tells the reader that the files will begin with 200 and end with 1000 and step by 200:

/scratch/data/ensight/avus/mach6/mach6_5.grd
/scratch/data/ensight/avus/mach6/mach6_5.bc
/scratch/data/ensight/avus/mach6/file????.pix
200 1000 200

Limitation

This reader does not support restoring EnSight Context Files.

Read Data

This reader inputs the format from the Barracuda solver by Computational Particle Fluid Dynamics (CPFD). This data traditionally has a large number of changing particle points within a static geometry composed of 2D walls and 3D fluids. This reader optimizes the geometry to only reload the particles each timestep, therefore improving performance.

GMV.xxxxx files contain the transient data where x is a digit (0-9) representing the timestep. In addition, there are a number of .gmv files, some of which must be present in the folder with the .gmv files: 00cells.gmv, 00drawcells.gmv, 00gridstl.gmv, 00mat.gmv, 00nodes.gmv, and 00poly.gmv. The 00gridstl.gmv file can be read separately to view the STL geometry (no variable, fluids, nor discrete particles), and the 00poly.gmv can be read separately as well to view the 2D polygon geometry (no variable, fluids, nor discrete particles).

Visit http://cpfd-software.com/ for more information about this solver.

Simple Interface Data Load

Load your geometry file using the Simple Interface method and trust that the translator will recognize the file type using the suffix.

Advanced Interface Data Load

For more options, load your geometry using the Advanced Interface method and click on the Format options tab as described below.

Data Tab
Format	Use the Barracuda format.
Set File	Select any one of the transient files (for example, GMV.00000) and click this button and all of them will be loaded.
Format Options Tab
Set measured	Select the measured file and click this button.
Reader GUI
Include Polygon Parts	Include polygon parts will include parts with polyhedral and/or polygon elements. Default is off.
Read Single GMV File	Toggle this On to read only the file you have selected and only the timestep represented by this file will be available. If off, this will read all the GMV files as a transient dataset, when you select only one. Default is off.
Console Output	Normal - Minimal console output, only for errors. Verbose - Normal output plus information about the model. Debug - Full information for the developer to diagnose a problem. Use this output to help to diagnose a problem or to send it to Ansys.

Read Data.

The CFF Reader is supplied compiled on Linux platforms on as as-is basis, and Ansys does not warrant nor support its use. A README file as well as the source code is also supplied with the EnSight distribution in the directory below.

$CEI/ensight251/src/readers/cff

Reads a CFX results (.res) file. Currently reads version 16.1-0 and earlier.

Simple Interface Data Load

Load your geometry/results file (typically named with a suffix .res) using the Simple Interface method.

Advanced Interface Data Load

Load your geometry/results file (typically named with a suffix .res) using the Advanced Interface method to customize the read, for example to read transient geometry (see below).

Data Tab
Format	Use the CFX-5 format.
Set file	Select the geometry/results file (.res) and click this button
Format Options Tab
Set measured	Select the measured file and click this button.
Reader GUI
Variable User Level	Allows you control of a number of variables read based on a call into the CFX API. The allowable choices are as follows: Level 0 - Read in all variables Level 1 - (default) Level 2 - Level 3 -
Variable Boundary Correction	Variable values are corrected using a boundary value correction if this toggle is Yes. YES - (default) Variable values adjusted using a boundary value correction. No - Variable values are not corrected.
Read Regions?	YES - Read regions. This is the default. No - Do not read regions. Note:  For 2022 R2, we have changed the default for Read Regions to YES. This change was made to improve the ability for the Turbo surfaces initialization, allowing the needed part separation which is not always available with the boundary specification (Read Regions is set to No). If you experience a regression in part creation due to this change, you can change Read Regions back to No. You can set this preferences in the Format dialog for future use.
Transient Geometry?	A flag to the reader if the data is transient. Note:  By default, a transient .res file will fail to load unless this is changed to Yes. CFX transient data will have a .res file and a series of .trn files (one for each timestep) located in a subdirectory. The res file will have the names of the .trn files, the time value and path. If the data is changing variables only then the .trn will not contain the mesh. If the mesh is moving, then you must turn on the Include Mesh in the Transient Result options so that the solver will write mesh information to each .trn file. Failure to do this results in a static, unmoving mesh over time. No - (default). Yes - Coordinates only.
Particles as Part?	If this is Yes, then EnSight reads in the particle data as a separate EnSight point part. No - (default) Do not read in particles as a separate EnSight Part. Yes - Read in the particles as a separate EnSight part

Caveat

Elemental values of Overset variables will be available only on Overset cell zones and boundaries attached to them.

Limitations

The CFX reader does not support Polyflow Classic data.

The CFX solver does export to EnSight Case Gold format.

CFX-Pre expressions that are saved during the simulation may show up in EnSight, otherwise expressions can be calculated within EnSight's calculator.

Variables that end in _beta have no units (for example, *_beta).

EnSight contains limited turbomachinery capabilities that are available in Beta. To have more details on this, see Ansys EnSight Beta Features.

Transient Blade Row (TBR) CFX model data is not supported in EnSight.

EnSight does not support a CFX multi-configuration simulation; the resulting .mres is not a recognized EnSight reader file format and reading should not be attempted. However, you can directly read the .res file(s) in the simulation subdirectories.

See Read Data.

Legacy Reader

There are three CGNS readers in EnSight: this one, the CGNS-XML Reader, and a legacy, unsupported reader (CGNS-Legacy) which is unavailable by default, but can be made visible in the list of readers in the data section of the preferences.

Some information on this reader is available at:

$CEI/ensight251/src/readers/cgns/README.txt

Simple Interface Data Load

Load your geometry/results file (typically named with a suffix .cgns) using the Simple Interface method.

Advanced Interface Data Load

Load your geometry/results files (typically named with a suffix .cgns) using the Advanced Interface method.

Data Tab
Format	Use the CGNS format.
Set cgns	Select the geometry/results file (typically .cgns) and click this button. For models contained in multiple files, wildcards or a special executive file can be used here. See Special Notes.
Format options tab
Set measured	Select the measured file and click this button.
	Include any Element sets defined. These are sets of full elements which are generally some logical subset of the total number of elements. Default is on.
Include Face/Edge Set Parts	Include any Face or Edge sets defined. These are some logical set of particular faces and/or edges of full elements. Default is on.
Include NodeSet Parts	Include any Node sets defined. These are generally the subset of nodes needed for the Element, Face, or Edge sets above. As such, they are generally not needed as separate parts, but can be created if desired. Default is off.
Include local elem res comps (if any)	Include the local stresses components, etc that are in the element's local system. A simple example is a bar (such as a truss element), which only has tension or compression in the element's axial orientation. Such an element would have an axial stress variable. Other elements would have appropriate result component variables. Default is on
Include Tensor derived (VonMises, etc.)	For tensor results, calculate scalars from the following derived results (principal stress/strains, and common failure theories): Mean Equal Direct VonMises Min Principal Octahedral Mid Principal Intensity Max Principal Max Shear By default, all 9 of these will be derived. You can control which are created by this toggle, with an environment variable. Namely, setenv ENSIGHT_VKI_DERIVED_FROM_TENSOR_FLAG n where n = 1 for Mean only 2 for VonMises only 4 for Octahedral only 8 for Intensity only 16 for Max Shear only 32 for Equal Direct only 64 for Min Principal only 128 for Mid Principal only 256 for Max Principal only 512 for all or any legal combination. example: for VonMises and Max Shear only, use 18. Default is on.
Regular Part Creation Convention	Parts will be created according to the following:
	Use Part Id	Part Id (this is the default)
	Use Property Id	Property Id
	Use Material Id	Material Id
Element Vars as	Single element values	Element results (whether centroidal or element nodal) will be presented as a single value per element. Therefore will be per_elem variables in EnSight. This is the default.
	Averaged to node values	Element results (whether centroidal or element nodal) will be averaged to the nodes without using geometry weighting. Therefore will be per_node variables in EnSight. This is a global averaging, so shared nodes are affected by all parts that share a node.
	Geom weighted average to node values	Element results (whether centroidal or element nodal) will be averaged to the nodes using geometry weighting. Therefore will be per_node variables in EnSight. This is a global averaging, so shared nodes are affected by all parts that share a node.
	Ave to node values <by parts>	Element results (whether centroidal or element nodal) will be averaged to the nodes without using geometry weighting. Therefore will be per_node variables in EnSight. This is a local averaging, so all averaging is contained within each part.
	Geom weighted ave to node <by parts>	Element results (whether centroidal or element nodal) will be averaged to the nodes using geometry weighting. Therefore will be per_node variables in EnSight. This is a local averaging, so all averaging is contained within each part.
Spatial Decomp Multiple File Search	Normally, a single CGNS file is specified and read. Namely, the model is neither decomposed spatially into more than one file, not temporally into more than one file. Therefore the first option is the default. However, when a model is spatially decomposed, it can be read as long as it conforms to one of the other three options below. Note:  This is not for temporally partitioned data. See Special Notes
	Use file specified	Opens only the file you specify. This is the default.
	Numbered in same dir	Opens and combines data from all filenames with the same pattern, but different ending numbers, that are in the same directory. file.cgns.1 <= specify this one file.cgns.2 ... file.cgns.9
	Same name in numbered dirs	Opens and combines data from all filenames with the same name, but in different numbered subdirectories. dir1/file.cgns <= specify this one dir2/file.cgns ... dir9/file.cgns
	Numbered in numbered dirs	Opens and combines data from all filenames with the same pattern, but different ending numbers, that are in different numbered subdirectories. dir1/file.cgns.1 <= specify this one dir2/file.cgns.2 ... dir9/file.cgns.3
Doing Structured as:	Structured	will cause originally structured parts to be created as structured parts in EnSight. This is the default.
	Unstructured	will cause originally structured parts to be created as unstructured parts in EnSight.
Var naming convention	Use Content Field (if provided)	Variable names will be what is in the Content field, if provided. If not provided, they will be the VKI dataset name. This is the default.
	Use VKI dataset name	Variable names will be the VKI variable dataset name (which are reasonably descriptive).
If Sections, which:	Which section will be used to create the variable
	First	The first section will be used (this is the default)
	Last	The last section will be used
	Section Num (below)	The section number entered in the field below will be used
	Separate Vars per Section	A separate variable will be created for each section.
If Section Num, 1-based integer value:	If the previous option is chosen to be Section Num, then the value in this field is the 1-based section number to use to create the variable.

Special Notes

Special file input methods for temporally decomposed models. Namely, a file per timestep. Possible file input methods:

You would need to either copy the .cgns file in the subdirectory to the data directory, or you will need to create a subdirectory for each .cgns file in the data directory, and move the .cgns files into those subdirectories. You could obviously take advantage of symbolic links to avoid actually moving any data.

Your other alternative is to use method 3) below.

However, having said that, there is one special case where you can use this method with the final file not being in the pattern subdirectories.

Special case requirements:

See Read Data.

Reads a Spymaster .spcth file.

See the following file for current information on this reader.

$CEI/ensight251/src/readers/cth/README.txt

Simple Interface Data Load

Load your geometry/results file(s) (typically named with a suffix .spcth) using the Simple Interface method.

Advanced Interface Data Load

Load your geometry/results files (typically named with a suffix .spcth) using the Advanced Interface method.

Data Tab
Format	Use the CTH format.
Set spcth*	To read one Spymaster file, put the CTH Spymaster file (typically named something filename.spcth) into the (Set) Geometry field. To read in multiple, related CTH Spymaster files (for example several files solved in parallel) as follows: filename.spcth.0 filename.spcth.1 filename.spcth.2 Put an asterisk '*' in the filename (filename.spcth.*).
Format Options Tab
Set measured	Select the measured file and click this button.
Reader GUI	User controls as shown below are available:
SOS Auto-distribute	When running EnSight in SOS mode, turn this ON (default) to tell the reader that you want it to intelligently distribute the data among the servers. Turn it off if you have already distributed the spcth files into different directories, or on different machines and want to use a Case SOS file to assign the spcth file(s) to EnSight Server(s) manually.
Open files one at a time	When running EnSight in SOS mode, turn this ON to tell the reader that you want it to only open one of the spcth files at a time. When this is OFF (default) every server process may open a number of the files simultaneously. This could be a problem if you have a thousand files and a thousand servers and your process reaches a limit with too many files opened at once.
Use Ghosts	Ghosts are invisible elements between the Server geometries that allow for interpolation of data results rather than extrapolation. Ghosts can be inner (default) - use only the inner ghosts between blocks all - use both inner as well as ghosts around blocks none - no ghosts normal - read in ghosts as normal cells. outer zero - read in the inner and outer, but zero the variable values on the outer locations. This is useful to create end caps on the isosurfaces.
Console Output	Normal - Normal console output Verbose - Extra output useful to the user to understand their data better. Debug - Extra output often useful in debugging problems.
(Set) Params	Allows user to enter parameters to change the behavior of the reader, often for debugging purposes. For example to limit the number of blocks in the part to 102, enter the following: -numblocks 101

Special Variables

EnSight's CTH reader has several special variables useful for understanding SOS data. FILE_ID is the file ID number for each cell. BLOCK_ID is the block index. And SERVER_ID is the server that has the data.

SOS details

You can start up SOS using enshell, or the legacy Case SOS file, or the legacy resources file (.res) file, each discussed elsewhere in this manual.

Reader-distribute is the default behavior of EnSight. In Reader Distribute mode, if you have more files than servers, files are distributed to servers in a round-robin fashion according to file size to even the load. If you have more servers than files, servers are allocated to files according to total file size per server. In Reader Distribute mode, all files must be available to all servers.

Shown below are graphical user interface images showing sample user input for a sample SOS read of 8 spatially distributed spcth files into EnSight SOS using a resource .res file.

If you decide that you want to manually distribute the files, then you must move the sets of files into separate directories, create the SOS case file with different directories and the filename* casefile, and toggle the reader SOS auto-distribute OFF in the Format Options above.

See Problems for more tips problem-solving your SOS visualization.

See Read Data.

The DVS reader reads in either in-situ data coming from a running solver or from a previouisly written cache. When running in-situ it can also optionally write the cache of data to be read in later.

This reader currently supports all EnSight element types for unstructured data. For structured data it accepts parallelepiped and curvilinear data.

It currently only supports scalar and vector variables (no complex or tensors yet).

When a cache is written the data will be split into multiple folders based on the number of EnSight servers it was written with. Each of these folders contains a sqlite database for metadata along with a hdf5 file containing the payloads of data received.

DVS Files

To be able to use the in-situ connection, a DVS file must be provided an example of contents are below:

#!DVS_CASE 1.0
SERVER_PORT_BASE=50055
SERVER_PORT_MULT=1
CACHE_URI=hdf5://localhost/D:/temp/testing_no_ensight

The initial #!DVS_CASE 1.0 should be provided to tell us what version of the file you are using. Currently, 1.0 is recognized.

SERVER_PORT_BASE: This should be set to a starting port for servers to listen for incoming data.

SERVER_PORT_MULT: This is used when running EnSight in SoS mode with multiple servers. It is used to increase the port number for each server sequentially. I.E. 1 means ports 50055, 50056 etc. 2 would be ports 50055, 50057, etc. 1 should be fine in most cases.

CACHE_URI: If this is not present, data will be in memory only. If it exists with a location, a cache will be written to that location if possible.

This is the format: <cache_domain>://<machine>/<location>

Limitations

Simple Interface Data Load

Load your DVS file using the Simple Interface method.

Advanced Interface Data Load

Load your DVS file using the Advanced Interface method.

Misc Notes

The Exodus reader links to the exodus routines in libexoIIc.a and the netcdf routines in libnetcdf.a. You must have these libraries to compile and run the ExodusII reader, and they are installed with EnSight.

Variable names that end in x, y, z will be treated as components of a vector. For example, the variables vel_x, vel_y, vel_z will be treated as a vector named vel_vec. Case is ignored in matching variable names.

GUI Control of Reader

Reader behavior can also be controlled in the Data Reader GUI via check boxes and fields. The environment variables, if set, are used to set the default values for the GUI.

Summary

Selecting the first file of any multi-file Exodus dataset will cause the reader to load the entire dataset. Selecting a non-first file of a spatially decomposed or a temporally decomposed dataset will cause the reader to load only that file. If you want to load only the first file, the Read Selected File Only toggle must be turned ON and that file selected. If a dataset is both spatially and temporally decomposed and a non-first file is selected, only the selected spatial decomposition will be loaded and it will be loaded for all time steps.

Single File - No Decomposition

If the file is not decomposed spatially nor temporally, then you will have only one Exodus file. Selecting this file will load all of the geometry and variables over all time. The file will be named something like file.e.

Spatially Decomposed Files

If the files are decomposed only spatially as shown below (each file contains a portion of the geometry over all time), then EnSight will behave as follows:

Temporally Decomposed Files

If the files are decomposed only temporally as shown below (each file contains all the geometry but only for a subset of the total time), then EnSight will behave as follows:

Spatially and Temporally Decomposed Files

If the files are decomposed spatially and temporally, as shown below, then there is a portion of the geometry in each file (indicated by 4.0, 4.1, 4.2, and 4.3) and a portion of the total time range in each file (indicated by s0002, and s0003) as shown below. EnSight will behave as follows:

Advanced Multiple File Naming

This reader supports two extensions to the filename fields. The first supports Exodus datasets where the geometry changes at some point in time. In this case, a new Exodus file (or set of files), is used for each set of solution times. To support this feature, insert wildcard characters (for example, * and ?) in the filename that expand to the name of the first files in each timeset.

The second extension allows for multiple files to be read as part of the same timeset (for example, domain decomposed files). This feature takes the form of a tag (<X:Y>) appended to the filename. The value of "X" is the number of files in the timeset and "Y" is the sprintf () format string on the integer (%d) formatting options) for expanding an integer argument into a string. http://en.wikipedia.org/wiki/Printf#printf_format_placeholders

For example, if a dataset consists of the following files:

Times 0-10 Times 11-15

Where the foo.e.* files contain timesteps 0 through 10 and the foo.e-s0002.* files contain timesteps 11 through 15. Also, each timeset is spatially decomposed into 3 subfiles, which each contain some portion of the dataset for the given timesteps. For this dataset, use the file pattern foo.*.03.<3:%0.2d> to tell EnSight there are multiple timesets and to generate the filenames for each timeset by replacing the <..> substring with a number from 0 to 2 as generated using sprintf() and %0.2d.

More Info

See the following file for current information on this reader.

$CEI/ensight251/src/readers/exodusII/README.exodus

Simple Interface Data Load

Load your geometry/results file (typically named with suffix .e, .ex0, .ex, or .ex2) using the Simple Interface method.

Advanced Interface Data Load

Load your geometry/results file (typically named with suffix .e, .ex0, .ex, or .ex2) using the Advanced Interface method.

Data Tab
Format	Use the Exodus II format.
Set exo	Select the geometry/results file (typically .ex1 or .ex2, or .ex0) and click this button. If there are multiple Exodus files in the solution set, select the first file to load all of the data.
Format Options Tab
Set measured	Select the measured file and click this button.
Reader GUI	When you choose Exodus reader, and toggle on the Advanced interface button, then click on the format options tab, you will see a number of options for controlling the reader behavior. Each of the choices in the data reader dialog has a corresponding Environment variable described below that you can set to control the default behavior. If you find yourself repeatedly toggling on or off choices in the Format options tab of the data reader dialog, consider setting specific Environment variables to change the default behavior of the reader.
Read Distribution Factors	Sets in Exodus can have distribution factor weights. If this is ON (default ON) then distribution factors will be read in as variables defined only on Set parts. The Environment variable ENSIGHT_EXODUS_DF can be used to set the default value (1 is ON, 0 is OFF).
Read Side Sets	Toggle ON (default) to read Side set parts. The Environment variable ENSIGHT_EXODUS_READ_SIDESETS can be used to set the default value (1 is ON, 0 is OFF).
Read Node Sets	Toggle ON (default) to read Node set parts. The Environment variable ENSIGHT_EXODUS_READ_NODESETS can be used to set the default value (1 is ON, 0 is OFF).
Read Element Sets	Toggle ON (default) to read Element set parts. The Environment variable ENSIGHT_EXODUS_READ_ELEMENTSETS can be used to set the default value (1 is ON, 0 is OFF).
Read Face Sets	Toggle ON (default) to read Face set parts. The Environment variable ENSIGHT_EXODUS_READ_FACESETS can be used to set the default value (1 is ON, 0 is OFF).
Read Edge Sets	Toggle ON (default) to read Edge set parts. The Environment variable ENSIGHT_EXODUS_READ_EDGESETS can be used to set the default value (1 is ON, 0 is OFF).
Read node and element maps	Toggle ON (default) to read node and element ids or labels (referred to in Exodus as node maps or element maps). There is no guarantee (particularly if using spatially decomposed Exodus files) that the node and element labels will be unique. If this option is toggled OFF then EnSight will ignore the labels in Exodus file and generate an internal numbering scheme guaranteed to have unique node and element ids. The Environment variable ENSIGHT_EXODUS_USE_NODEMAPS can be used to set the default value (1 is ON, 0 is OFF).
Verbose Mode	Toggle ON (default OFF) to output more detailed information to the server console. The Environment variable ENSIGHT_EXODUS_VERBOSE can be used to set the default value (1 is ON, 0 is OFF).
Read higher order elements	Toggle ON (default ON) to preserve higher order elements. Toggle OFF to down convert these elements to simpler elements (for example, convert a HEX20 into a HEX08). The Environment variable ENSIGHT_EXODUS_USE_HIGHERORDERELEMENTS can be used to set the default value (1 to preserve higher order elements and to 0 to convert these elements to simpler elements.
Read constant variables	Toggle ON (default ON) to load the variables that have a single value at each timestep (called Constants in EnSight). The Environment variable ENSIGHT_EXODUS_READ_CONSTANTS can be used to set the default value (1 to load constant variables and 0 to not load them).
NAN filter input data	Toggle ON to check all floats (geometry as well as variables) for IEEE nans and set to zero if nan (default ON). The Environment variable ENSIGHT_EXODUS_CHECK_NANS can be used to set the default value (1 to check all floats and 0 to not check floats).
Clip Overlapping timesteps	EnSight must have monotonically increasing time values in each successive timestep. Exodus files sometimes have overlapping timesteps. Toggle this ON, and when overlapping times are encountered, EnSight will truncate the former values and use the latter timesteps to construct the timeline. If this is toggled OFF (default) and EnSight encounters duplicate time values in subsequent timesteps it will apply the epsilon value (see Epsilon below) and increment the latter timestep so it remains monotonically increasing. With this option toggled OFF, EnSight will retain all timesteps but change the time values and is therefore not recommended. The Environment variable ENSIGHT_EXODUS_CLIP_TIMESTEP_OVERLAP can be used to set the default value (1 to truncate the timesteps with overlapping time ranges, and 0 to keep all timesteps).
Epsilon	A delta time value (default 1.0) to be substituted when a non-increasing delta time float value is encountered. If the reader detects two sequential time values that are not increasing the later solution time value will be set to the earlier time plus this epsilon value. This will have a cascading effect, shifting other solution times later as well. This is useful when the solution times are all the same value in the Exodus dataset. Set the Environment variable ENSIGHT_EPSILON to a positive float value to change the default value.
Read Selected File Only	Toggle ON to read one and only one file which is the selected file. Toggle OFF (default) to allow automatic pattern recognition (and loading) of certain categories of file naming schema as discussed in the beginning of this section. ENSIGHT_EXODUS_READ_SELECTED_FILE_ONLY can be used to set the default value (1 to read only one file and 0 to read all matching files in the schema).
Use Undef value for missing variables	Toggle ON (default) to return EnSight's undefined value when missing variable values are encountered (see EnSight Gold Undefined Variable Values Format ). Toggle OFF to return a value of 0.0 for missing variable values, which is the behavior of the reader prior to reader version 2.72). The Environment variable ENSIGHT_EXODUS_USE_UNDEF_VALUE can be used to set the default value (1 to return UNDEF and 0 to return 0.0 for missing variable values).
Read element attribute vars	Some elements have unique attributes (such as thickness for 2D shell elements). Toggle ON (default) to read in element attribute variables and OFF to not read these in. Use the Environment variable ENSIGHT_EXODUS_READ_ELEMENT_ATTRS to set the default value (1 to read these values 0 to not read them).
Use detected DTA XML file	Toggle this ON (default is OFF) to check for the existence of a .dta file (and read it in). The DTA file has extra metadata more fully describing the parts. Set the Environment variable ENSIGHT_EXODUS_USE_DTA_FILE to change the default (1 is read .dta file, and 0 is do not check).
Auto generate DTA XML file	Toggle this ON (default is OFF) to generate a stub .dta file from the Exodus datafile. Set the Environment variable ENSIGHT_EXODUS_AUTOGEN_DTA to change the default (1 generate stub .dta file, 0 is do not generate .dta file).
Read part names	Toggle this ON (default is ON) to read in the part names from the Exodus data file. Set the Environment variable ENSIGHT_EXODUS_USE_FULL_NAMES to change the default (1 to read in the part names from the Exodus data file, 0 to not read them in).
Assume unchanging connectivity	By default, with this Toggle OFF, when an Exodus dataset has multiple temporal files, the reader assumes that this is a changing connectivity file. Changing connectivity geometries lose some capabilities within EnSight, such as the ability to interpolate variable values between timesteps. If you know your temporally decomposed dataset does not change connectivity, then toggle this ON to tell EnSight to not make this a changing connectivity dataset; the dataset will become a changing coordinates geometry (which does allow interpolation between timesteps). To change the default, set the environment variable as follows: ENSIGHT_EXODUS_ASSUME_UNCHANGING_CONNECTIVITY to a value of 1 and the toggle will appear ON.
Scale Factor	Enter a positive float value (default 1.0) to be used as a scale factor for geometry and vectors (not for scalars). Set the Environment variable ENSIGHT_EXODUS_SCALE to a positive float value to change the default value.
Max time steps	By default, EnSight can read from an Exodus file while the simulation code is updating the Exodus file. For allocation purposes, EnSight needs an absolute maximum number of steps that will appear in the data file(s) during your EnSight session. Currently, the maximum number of time steps that EnSight will read is given here as 100000. Increase this value if your solver may exceed this amount. A value less than or equal to 1 will disable the ability to check for new time steps. Note:  This field is ignored on Exodus files with HDF5 as the underlying format, as HDF5 files cannot safely be read and written simultaneously. Set the environment variable ENSIGHT_EXODUS_MAX_TIMESTEPS to change the default. For details on how to use this capability in EnSight, see How To Change Time Steps and the Advanced section in How To Load Transient Data).

SOS

You can start up SOS using enshell, or the legacy Case SOS file, or the legacy resources file (.res) file, each discussed elsewhere in this manual.

There can be no more servers than the number of sub-files however (but fewer servers are legal and in most cases, recommended). Finally, if there are sub-files, the number and the naming convention must be the same over all timesets.

The Exodus reader does the decomposition automatically when running in Server of Server (SOS) mode, which is called Reader-distribute mode. In Reader Distribute mode, data is distributed to servers in a round-robin fashion. In Reader Distribute mode, all files must be available to all servers.

If you decide that you want to manually distribute the files, then you must move the sets of files into separate directories, create the SOS casefile with different directories and the filename* casefile, and toggle the reader SOS auto-distribute OFF in the Format options above.

Shown below are graphical user interface images showing sample user input for a sample read of spatially distributed Exodus files (4 processors) into EnSight SOS using a simple 4-server resource (sos.res) file as follows. Also shown is the geometry colored by the Server number calculated using the Calculator Function ServerNumber (which is an excellent way of showing the allocation of the geometry among the EnSight Servers. See the Problems section of the Use Server of Servers for more tips problem-solving your SOS visualization.

#!CEIResourceFile 1.0

SOS:

host: localhost

SERVER:

host: localhost

host: localhost

host: localhost

host: localhost

See Read Data.

A FIDAP Neutral file contains all of the necessary geometry and result information for use with EnSight.

A neutral file is produced by a separate procedure defined in the FIDAP documentation. If the data is time dependent this information is also defined here.

Simple Interface Data Load

Load your geometry/results file (typically named with a suffix .fdneut) using the Simple Interface method.

Advanced Interface Data Load

Load your geometry/results file (typically named with a suffix .fdneut) using the Advanced Interface method.

See Read Data.

This EnSight reader uses the FLSGRF READER API LIBRARY from FlowScience in order to read data from a Flow3D flsgrf* output data file as well as the prpgrf* files written out in preprocessor mode (which contain only one timestep). FlowScience is no longer supporting compressed formats with the *.fgz and *.dat suffix.

Requirements

If any extra FlowScience API debug files are desired from the EnSight session, the FLSGRF API requires that the user have write permissions in the directory where the flsgrf file resides.

THE FLSGRF API is only available for Windows 32-bit, 64-bit, Linux 32-bit, and Linux 64-bit platforms.

EnSight attempts to implement the latest FLSGRF API and the FLSGRF API should read flsgrf files written by older versions of Flow3D.

Data Types

There are several kinds of data available in a Flow3D flsgrf output file, each with its own EnSight timeset: Restart, Selected, Fixed, and Particle data.

Restart Data

By default, there are 11 restart timesteps per solution: t=0 and an additional ten each spaced at 1/10th of the total simulation time. You can change this frequency in Flow3D using the plotting interval (PLTDT) in the PREPIN input file.

Selected Data

This consists of selected variables output at a higher number of timesteps. Restart and selected data can both be available in the data file.

Fixed Time Group

This data does not change over time. It consists of simulation parameters such as binary flags used to activate physical models as well as mesh data.

Parallel Solution

If multiple flsgrf files (flsgrf1.dat, flsgrf2.dat, ...flsgrfn.dat) from a parallel run and the number of servers equals the number of files, then choose the first one (flsgrf1.dat) and choose decomposition spatial and the remainder will be automatically loaded. Each server reads only one of the spatially decomposed files therefore dividing up the memory requirements. For temporal decomposition, load all the spatially decomposed files flsgrf*.dat and choose temporal decomposition. In this mode, each server loads a separate timestep therefore speeding up transient post-processing.

Particle Data

If particles are present in the simulation they will be present in the Restart data. If you request particle information in the Selected data (from their project file where anmtyp(i)='part') then particle information will also be available in the Selected data timesets.

Particle data is not imported into EnSight by default. To import this data, Choose the Multipart Flow3d reader then click on the Format options tab and select the type of Particle data that you wish to import.

Geometry is STATIC in EnSight unless Particle data is imported and then the geometry is CHANGING CONNECTIVITY because the number of particles can change with each timestep.

Technical Notes

All block part variable data is cell-based (per element data). All particle variable data is node-based (per node data). All FSI/TSE data is node-based (per node).

To visualize the fluid in the block try creating an isosurface of the Fluid Fraction using an isosurface value of 0.51. Now to see the surrounding structure, make another isosurface with a value of 0.51 using the Cell_Volume_Fraction_Fixed variable. Click on the paint can icon and change your shading to smooth to improve the isosurface look. To see the fluid as an isovolume, File → Command and type in test: simple_isovolume_off then make an isovolume from 0.5001 to 1.0 using the Fluid Fraction and again change its shading to smooth.

To see detailed information about variables, blocks, boundary conditions, etc., choose Console Output Debug as described below.

This reader makes use of Timesets. Each of the variable types has it's own Timeset timeline and EnSight merges them all together. For details on using these timesets see the advanced section of the Change Time Steps in the Ansys EnSight How-To Manual.

Ghost Cells

Ghost cells are invisible elements that help EnSight to interpolate variable values. For example, Ghost cells between blocks allow for a smooth transition of the isosurface of the fluid surface at part block boundaries. Ghosts that are not used have a zero value for the variable, and must be removed: removal of ghosts at a symmetry surface allows for smooth mirroring of the part(s).

Units

If the units are specified in a known unit system in the data file, then EnSight can convert them to any of the other known unit systems at read in. Also, EnSight can annotate by the units for any of the variables (those not non-dimensionalized).

Updated Info

$CEI/ensight251/src/readers/multi_flow3d/README.txt

Simple Interface Data Load

Load your Flow3D file (typically named flsgrf*) using the Simple Interface method.

Advanced Interface Data Load

Load your Flow3D file (typically named flsgrf*) using the Advanced Interface method.

Data Tab
Format	Use the Flow3d-Multiblock format.
Set flsgrf	This field should be an flsgrf or prpgrf file. If multiple flsgrf files (flsgrf1.dat, flsgrf2.dat, ... flsgrfn.dat) from a parallel run, then choose all using an asterisk (flsgrf*.dat) in place of the numbers, or one by specifying the particular file (flsgrf1.dat).
Format Options Tab
Format Options
Rename Variables	Variables are renamed by default to be easier to interpret for Flow3D users.
Include Symmetry Ghosts	Flow3D includes the following boundary conditions: symmetry, wall, continuative, periodic, specified pressure, specified velocity, grid overlay, outflow and interblock. Ghosts are always included in periodic, specified pressure, and inter-block boundary conditions. Ghosts are optional (using a toggle) for the following boundary conditions. symmetry - include symmetry ghosts toggle wall - include wall ghosts toggle other - (continuative, specified velocity, grid overlay and outflow) - include other ghosts toggle. By default, symmetry ghosts are removed so that mirroring in EnSight has no seam. However toggling ON this flag will include the symmetry ghosts for example for inviscid flow using the symmetry condition to simulate a wall.
Include Wall Ghosts	Flow3D includes the following boundary conditions: symmetry, wall, continuative, periodic, specified pressure, specified velocity, grid overlay, outflow and interblock. Ghosts are always included in periodic, specified pressure, and inter-block boundary conditions. Ghosts are optional (using a toggle) for the following boundary conditions. symmetry - include symmetry ghosts toggle wall - include wall ghosts toggle other - (continuative, specified velocity, grid overlay and outflow) - include other ghosts toggle. By default, wall ghosts are removed so that the EnSight fluid/wall interface does not show up using the isosurface of the fluid fraction. However toggling ON this flag will cause the fluid/wall interface to show up using the isosurface of the fluid fraction.
Include Other Ghosts	Flow3D includes the following boundary conditions: symmetry, wall, continuative, periodic, specified pressure, specified velocity, grid overlay, outflow and interblock. Ghosts are always included in periodic, specified pressure, and inter-block boundary conditions. Ghosts are optional (using a toggle) for the following boundary conditions. symmetry - include symmetry ghosts toggle wall - include wall ghosts toggle other - (continuative, specified velocity, grid overlay and outflow) - include other ghosts toggle. By default, these other ghosts are removed so that the EnSight fluid/wall interface does not show up using the isosurface of the fluid fraction. However toggling ON this flag will cause the fluid/wall interface to show up using the isosurface of the fluid fraction.
Read History Queries	The flsgrf file often includes xy plotting data in the form of history data that is loaded into EnSight as pre-defined Queries accessible by clicking on the Query/Plot icon or below the part list in the Parts/queries tab. Default is ON.
Load FSI TSE Parts	Fluid-Structure Interaction and Thermal Stress Evolution unstructured parts (hexa8 and tet4's) and their associated stress, strain, temperature, displacement and blanking (STATUS) nodal variables are loaded into EnSight by default. A TSE (thermal stress evolution) component is a region in the fluid, where the fluid solidified and a structural analysis is performed in the solid in response to thermal gradients. An FSI (fluid-structure interaction) components, is a solid region in the fluid where the flow-induced structural deformations in turn, influence the flow, requiring simultaneous structural and fluid flow solution There can be only one TSE part in a simulation.
Restart	Load the variables on the Restart Timeline. Default ON.
Selected	Load the variables on the Selected Timeline. Default OFF.
Particle Data	By default, particle data is not read into EnSight. Choose the appropriate timeline to read in the Particle data.
Console Output	Use this flag to determine the amount of output to the console. Normal - Usually only echo errors to console. Verbose - Normal output plus an echo of every Fluent part that is in the dataset, whether it is interior or not, whether it is skipped, what variables are defined for which parts, and to echo it's EnSight Part number. Debug - Verbose output plus more detailed output and progress through the reader routines often valuable for understanding and reporting problems. Also detailed block information, variable information, boundary condition information, and timeset information
Treat Ghosts	Ghost elements are invisible elements that help EnSight to interpolate variable values. Ghosts can be read in as Ghost cells, as normal (visible) cells, or they can be not read in at all. Ghosts - include invisible ghost elements according to the Flow3D boundary conditions (default) and user settings. None - Use NO ghost elements. This will especially be apparent in the gaps in the isosurface between data blocks due to the lack of these invisible interpolating elements. Normal - Use ALL ghost elements as NORMAL, visible elements. This is useful for understanding boundary conditions around part blocks.
Load Internal STL	The flsgrf file sometimes includes surface, boundary condition, or other important surface geometry on one or more timelines. Default is to load None, but the pulldown allows you to choose Selected, Restart, or Static STL geometry timelines.
FS Meta File Output	The FlowScience reader API, optionally writes out optional performance and debug files when a flsgrf file is opened if you have write permission. These can help to speed up reading the second time a file is opened or to understand the details of the read or to diagnose a failed read. However, if multiple users each with different file mask permissions attempt to open a flsgrf file on a shared network hard drive, the writing and overwriting of these files becomes problematic and can cause a read to fail. The safest option, if others may follow your read of a given file, is to choose to not write out these optional files. The API offers four options on opening a file named, for example, flsgrf: None - write out no additional files Performance - writes out c-flsgrf, flsgrdr, g_flsgrf, and t_flsgrf files. Debug - writes out the flsout.rdr file All - writes out both Performance and Debug files.
Units	Convert units to selected type. FlowScience reader API allows the conversion of a known system units (CGS, SI or English) to another known system (CGS, SI, or English). EnSight will not convert from an unknown or unspecified unit system. Unchanged (default) - use the system of units in the data file CGS - Uses grams, centimeters, and seconds. SI - Uses kilograms, meters, and seconds. English - Uses slugs, feet, and seconds.
Temperature Units	Temperature units are always known (C, K, F, or R) and can therefore always be converted to any other unit system. Celsius - Convert to Celsius Kelvin - Convert to Kelvin Fahrenheit - Convert to Fahrenheit Rankine - Convert to Rankine Unchanged (default) use the temperature units in the data file
Decomposition	If running in EnSight SoS mode, the type of decomposition to use. None - Spatial - Traditional SOS mode in which each server is assigned one of the spatially decomposed block files. Temporal - Temporal SOS in which the data is not spatially decomposed, but rather each of the available servers reads a different timestep to speed up transient post processing.
Set measured	Select the measured file and click this button.

Parallel Post Processing (SOS)

The Flow3D solver can calculate its solution in parallel. This type of solution writes out the data as separate files (flsgrf1.dat, flsgrf2.dat, flsgrf3.dat, ....), each containing one structured block. EnSight can read each of these files onto a separate server. Server 1 will read in the unstructured data plus block 1, server 2 will read in block 2, server 3 will read in block 3, etc.

You can create an SOS casefile (.sos), which maps out which server loads what data and start EnSight up in SOS mode, and just load the sos casefile directly. Alternatively, you can create a .res file to set up the servers, start up EnSight in SOS mode, and load the data as flsgrf*.dat, and, in the data reader dialog, choose the .res file and choose to allow sos to use the *. For more details (including a sample resource file and sample SOS case file and how to use them, see Use Server of Servers and search for Flow3D.

See Read Data.

You have three methods to bring the data from Fluent into EnSight :

Which one to choose:

In general and common use cases requiring generic post processing needs, pick your variables of interest and export Common Fluids Format (.cas.post/.dat.post). In EnSight, use the Ansys Post File reader to import the .cas.post/.dat.post files.

For large data, where parallel is needed for capacity, pick your variables and export EnSight Case Gold nodal.

If you want to have a look at the raw restart data, you can load cas.h5/dat.h5, but be aware that some of the dat.h5 variable values are raw values intended for Fluent restart.

The preferred method is reading Case Gold exported directly from Fluent (which also works in parallel for large solutions). But if using the Fluent reader then .cas and .cdat is the next best method because the variable values from the .cdat will be corrected in Fluent prior to export to .cdat and available on all parts and correctly exported from Fluent. While the .dat variable file is readable and usable by the Fluent reader, it contains variable data that is only useful within Fluent for restart purposes and may not be accurate on all parts.

See the following files for current information on the Fluent direct reader.

$CEI/ensight251/src/readers/fluent/README.txt

The comments that follow are for the current Fluent reader. The reader loads ASCII, binary single precision, or binary double precision. The files can be uncompressed or compressed using gzip.

Simple Interface Data Load

Load your geometry file (typically named with a suffix .cas) using the Simple Interface method.

Advanced Interface Data Load

Load your geometry and result files (typically named with a suffix .cas and .dat) using the Advanced Interface method.

Data Tab
Format	To use this reader, select the Fluent format.
Set cas	Select the geometry file (typically .cas or .cas.gz) and click this button. For transient data, use a single asterisk to replace the number (*.cas or *.cas.gz).
Set cdat, dat or fdat	Select the results file (typically .cdat or .dat or .dat.gz), and click this button. For transient data, use a single asterisk to replace the number (*.dat or *.dat.gz). Note:   .fdat files (see AIRPAK/ICEPAK Reader) are also usable in place of the .dat file. The .cdat file is the automatic selection, followed by a .dat. If a .cdat or .dat file is collocated with a .fdat file, you will have to manually select the .fdat file and then click the Set cdat, dat, or fdat button to use a .dat file variant.
Format Options Tab
Set measured	Select the measured file (typically a .mea suffix) and click this button. If you have fluent particle data you can translate it into EnSight's measured data format and import the particles as measured data.
Other Options using the current Fluent reader
Load Internal Parts	Toggle this ON to load the Fluent Internal Parts. This will show all the internal walls forming all the cell volumes. If you do toggle this on, then it is recommended that you click the Choose Parts button at the bottom of the data reader dialog, rather than Load all, as you'll only want to load the interior parts of interest to save memory and time. Default is OFF.
Use Meta Files	Meta files are small summary files that contain highlights of the important locations inside each of the Fluent files. Allowing the EnSight reader to write out Meta Files that map the locations of important data can provide a significant speed up the next time you access that timestep. It is recommended that you leave this toggle ON. If you have write permission in the directory where your data is located, three types of binary Meta Files will be written when you first access each file, with extensions .efc for the .cas file, .efd for the .dat file and .efg for the time-history data. They are optional, and if you don't have write permission, the reader will take the extra time to read the entire .cas and .dat file to find the relevant data each time you come back to that timestep.
Load _M1 _M2 vars	Variables that end in _M1 and _M2 occur in Fluent unsteady flow. They represent the value of the variable at the prior iteration time and the time prior to that respectively. By default this toggle is OFF and these variables are not loaded. Toggle this ON to load these variables.
Load all cell types	Fluent cells have a boundary condition flag. By default (toggle OFF) EnSight loads only the cells with a boundary condition flag equal to 1 (one). Toggle this option ON to load all cells with a non-zero boundary condition. For example, if you have a part with cells of boundary condition 32 (inactive), EnSight will, by default not load this part. Toggle this option ON and EnSight will load this part. Note:  Parts containing cells with a boundary condition of zero are never loaded.
Poly to Regular Cell	Fluent polyhedral cells when composed of the correct kind and number of regular faces can be converted to regular cells (tetrahedrons, hexahedrons, pyramids, or wedges) boosting EnSight speed and decreasing memory requirements. Toggle ON and reader checks each polyhedron to see if it can be converted to a regular cell (default) and OFF to not convert any polyhedral cells. There is very little slowdown during the read to do this and a big payoff for some datasets with large numbers of convertible polyhedra. Leave it on.
Poly faced Hex to Poly	Fluent hex cells that transition to a more refined hex mesh will sometimes have one or more of the quad4 faces subdivided into four quad4 faces. For example a hexahedral cell with one transition face will have the six full faces, and four subdivided faces for a total of 10 faces. Toggle ON and the subdivided faces are kept rather than the full face and the cell is changed into a polyhedral which will slow down EnSight performance, and greatly increase memory. The polyhedral also will have hanging nodes (see the next toggle). Toggle OFF (default) to convert the hex element to a six-sided hex which will be adjacent to four smaller cells rather than completely connected to them slowing down EnSight's adjacency searching. The default is thought to be the lesser of two evils.
Fix Hanging Nodes	Some Fluent polyhedral cells and all transition hex cells converted to polyhedrals will have hanging nodes. A hanging node is a node not shared by at least 3 faces. A polyhedral element with hanging nodes is not water tight and can cause real problems in EnSight, so it is best to leave this toggle ON (default) and only turn it OFF for experimental purposes.
Read Parallel CAS Variables	For parallel investigation, if the user toggles on read .cas variables, this option creates two new elemental scalars: ELEMENT_INDEX and PARTITION only if the data is solved in parallel and has partition section(s). This is primarily useful to visualize the Fluent geometric decomposition of parallel solutions.
Read Particle Variables	This will read particle coordinates and variable data from the .dat file. The number of particle parts is equal to the number of injections.
Use Zone IDs for Parts	A heterogeneous mix of serial and parallel solution files will result in a jumbled part ordering between CAS files. Toggle this ON to use the part zone id to reorder the parts consistently from .cas file to .cas file using the first file loaded as the canonical order.
Read all files to create variable list	Some transient datasets have different variables in the different .dat files. If this is OFF (default) then only the last .dat file will be used to create the variable list. If ON, then all .dat files will be used to create the master variable list. Regardless of the option, a variable will be assigned the EnSight Undefined value at time steps where it is undefined.
Console Output	Use this flag to determine the amount of output to the console. Normal - Usually only echo errors to console. Verbose - Normal output plus an echo of every Fluent part that is in the dataset, whether it is interior or not, whether it is skipped, what variables are defined for which parts, and to echo it's EnSight Part number. Debug - Verbose output plus more detailed output and progress through the reader routines often valuable for understanding and reporting problems.
Time Values	Use Filename Numbers will read the sequential numbers at the tail of the filenames and adjust them by making the first number 0 and shift all subsequent values. That is, file4000001.cas, file4000004 ... file4000020 is as follows: timestep 0 has time value 0.0, timestep 1 has time value 3.0, and timestep n has time value 19.0. Use Time Steps will make timestep and time value the same for example: timestep 0 will have time value 0.0 and timestep 5 have time value 5.0. Read Time Values (default) will open each file and find the exact time value using the 'flow-time' keyword. This means that every file has to be opened and searched. Failing that it defaults to the Calc Const Delta. Calc Const Delta reads a delta time from one file using 'physical-time-step' keyword, and calculates the time values by multiplying the delta value by the adjusted filename number. Failing that, it defaults to the Use Filename Numbers option. It is essential that your time values are correct for some calculations (for example, if you are going to do pathline tracing). Keep in mind that if your timesteps are uniform then you can use the 'Use Time Steps' option and just scale your time values using the Time Options tab in the data reader dialog. If your timesteps are not uniform, but your File Numbers are proportional to your timesteps then you can select Use Filename Numbers and then scale the time values using the Time options tab in the data reader dialog.

Node and Elem IDs

Parts have node and element ids to enable querying your data. Node ids are created from the coordinate global node. Element ids are created as follows. Face part elements are uniquely numbered according to their zone index. Cell part elements are uniquely numbered using their zone index added to the total number of faces. So a dataset with 100 face elements and 300 cell elements would have the face elements number 1-100 and the cell elements numbered 101-400. In Verbose mode, the element id range for each part are written to the console.

.CDAT File

The variables in the Fluent .dat file are restart variable values that may require Fluent algorithmic manipulation in order to see values reflecting the actual flow physics. EnSight is not equipped with the physics found in Fluent, therefore reading the .cas and the .dat results in variable values missing (e. g. symmetry plane is missing variables) or wrong (velocity vectors are not parallel to the symmetry plane, or no-slip wall velocity is undefined rather than zero). The workaround, from within Fluent, is to export the variable values into the .cdat file (Fluent applies the physics to the .dat variables and then exports them to the .cdat file(s)) for all the part(s).

The EnSight Fluent reader has been updated to support Fluent 19.2 .cdat files. To take full advantage of this improved capability, the Fluent user will select the Fluid Part(s) within Fluent and export all variables of interest into the .cdat file. This will export properly extrapolated elemental variable values for all the fluid(s) as well as all the surfaces defined from the fluids. The user will then enter the .cas and the .cdat file into the geometry and results fields, respectively in the data reader dialog. The .cdat is the preferred form for reading variable values and should be used at all times over the .dat file(s).

Because the variables from the .cdat file are potentially different than those from the .dat file, Fluent renames these variables from the .cdat file using lowercase text. Further, .cdat variables are always scalars; the Fluent reader currently reassembles velocity and wall shear vectors only, but some other vectors may be missing, showing up only as three scalar components. Users with old command files can continue to read the .cas .dat files which may continue to work (some special datasets that go from serial solution to parallel solution may have the part IDs reordered and won’t run correctly). Using a command file created with the .cas and .dat files on a .cas and .cdat will not work (nor will older context files restore) due to these variable name changes.

In addition, the CDAT format can be used to export surface geometry (walls, isosurfaces, clip planes, inlet parts, etc), to greatly reduce the size of the output and keep it tractable for post-processing and their corresponding nodal variables. If either surfaces or fluids are exported then the nodal or elemental variables exported will match the corresponding geometry, respectively.

However, if both the fluid and the user surfaces are exported together, then elemental fluid variables (with their normal names) and nodal user surface variables (named with prefix us_*) will be exported. The elemental fluid variables will be undefined on the user surface parts and the nodal user surface variables will be undefined on the fluid parts. This can cause confusion when working in EnSight. For example, if the user tries to use a boundary layer calculator function using on a user surface part, you must tell the function to use the velocity that is defined on the fluid part in order to make this calculation.

Variable Location

Variables that are cell-centered remain where they are found in the .dat file, that is the reader does not interpolate the cell-centered variables to the nodes. Fluent can export variable data to EnSight's Case Gold format at either the nodes (default) or at the elements (same as .dat file). Unfortunately older versions of Fluent export variables averaged to the nodes leading to flow into and out of walls which causes particles to stop prematurely and skews mass flow calculations. Later versions of Fluent consider boundary conditions prior to averaging the data to the nodes, yielding a much more realistic representation of the physics.

Variables Undefined

Not all variables exist on all parts in the .dat file. If you select a part and color by a variable and get undefined, then load the data using Verbose mode and take a look at the console. Your variable is probably not defined for this part and EnSight does not have the boundary conditions nor the solver physics algorithms to extrapolate variable values to boundary parts. Create a clip on the location of an interior part on a volume part if you want to see a plane with the values from the volume.

Extra Variables

EnSight will try to calculate extra CFD variables given the existing DAT variables for your convenience.

gzipped files

Files that are gzipped can be read by EnSight. However, with large numbers of parts this can result in a substantial slow down in the access of variable information in the .dat file because this involves non sequential access (seeking around various places in the file rather than sequentially moving through the file in order) which has been shown to result in dramatic slow downs. The workaround is to simply ungzip your files prior to reading them into EnSight.

CAS Constants

Extra CAS Single Value Variables - A number of single value variables are read from the .cas file(s). These will show up in the EnSight Calculator named as follows.

PRESSURE_ABS - operating pressure (absolute)

PRESSURE_ABS_INIT - initial operating pressure (absolute)

GAMMA_REF - reference gamma, ratio of specific heats

VISCOSITY_REF - reference viscosity

TEMPERATURE_REF - reference temperature

PRESSURE_REF - reference pressure

DENSITY_REF - reference density

SPEED_SOUND_FAR - far field speed of sound

PRESSURE_FAR - far field relative pressure

DENSITY_FAR - far field density

R_ref - Calculated reference gas constant = PRESSURE_ABS / (DENSITY_REF * TEMPERATURE_REF)

V_def - Calculated default velocity magnitude from x, y and z-velocity default values

M_def - Calculated from V_def / SPEED_SOUND_FAR

UDS, UDM Variables

UDM and UDS variables now read in as UDM_0, UDM_1, UDM_2... and UDS_0, UDS_1, .... Fluent differentiates between UDS (User defined scalar) and UDM (user defined memory) as follows.

A UDS is a scalar variable for which a transport equation can be solved (for example, transport of a red color from an injection nozzle into the volume; convective terms, diffusive terms,.) The single terms of this transport equation are programmed via UDF (user defined functions) in C and are run time libraries.

A UDM is a node-based value which also is calculated using a UDF (for example, viscosity against local temperature and density). For UDMs transport equations are not solved. Therefore they require less memory compared to UDS.

UDMs and UDSs are available for additional physics which are not available in Fluent (for example one can use a UDM for the calculation of dust concentration in filter elements.

Limitations

If species data is available only in Fluent PDF format, then the EnSight reader will not create the Mass and Mole fraction variables.

Polyhedral Elements

There are two methods to import polyhedral elements into EnSight. The first is to try using the direct reader. This has the advantage that the direct reader will attempt to convert polyhedral elements back to regular elements, saving memory and speeding up EnSight. The second is to export EnSight Case Gold .encas file from Fluent in parallel, decomposed format. Case Gold has the advantage of currently Server of Server in parallel, which can distribute the many tasks to multiple servers and speed up post processing (requiring an EnSight Enterprise license, formerly gold or hpc).

Periodic Elements

The reader now supports rotational symmetry to provide continuous boundaries.

Particles

The reader should attempt to read particles if they are present in the file(s).

Included with EnSight is a Fluent particle file translator to translate the Fluent .part file into an EnSight measured (.mea) data file. To get help with this translator, type $CEI/ensight251/machines/platform/flupart -h where platform is your hardware/OS architecture (for example, linux_2.6_64 or apple_10.5, win32, etc.).

Source code and README for this translator are locate $CEI/ensight251/translators/fluent/Particles/

This measured data file is entered in the measured data field under the Format options tab of the data reader dialog.

See Read Data.

Variable Names

The names of the variables are created within the EnSight reader using simply the ID of the variable found within the variable file (.dat) mapped to a reasonable text name found within the reader.  However some of the variables are unknown or internal to Fluent and therefore not named. The practice of this reader is to show all variables and therefore the variable internal name is used. For example, the variable SV_ARTIFICIAL_WALL_FLAG is an internal Fluent variable, and there is no text name. So this name is used.

The Fluent HDF5 reader is supplied with EnSight to read Fluent .cas.h5 and .dat.h5 restart files written in Fluent 2019 R1 and onwards. .h5 extension indicates that they are HDF5 files. This reader uses Ansys CFF SDK (R20.2) to read all the information from .cas and .dat HDF5 files. This reader relies entirely on CFF SDK to provide necessary information to create parts and variable list. Using the R20.2 SDK, some older files (circa 19.3-19.5) may fail to read. For those seen so far, reading them into Fluent 2020 R2 and saving again resolves the issue.

Simple Interface Data

Load Fluent geometry file (typically named with a suffix .cas.h5)

Advanced Interface Data Load

Load Fluent geometry and result files (typically named with suffix .cas.h5 and .dat.h5) using Advanced Interface methods.

Data Tab
Format	To use this reader, use Fluent_HDF5 format
Set .cas.h5	Select the geometry file (typically .cas.h5) and click this button. For transient dataset, use a single asterisk to replace the number (*.cas.h5)
Set .dat.h5	Select the result file (typically .dat.h5) and click this button. For transient dataset, use a single asterisk to replace the number (*.dat.h5)
Support to .msh.h5 file	Select the geometry file (typically .cas.h5) and click this button. For transient dataset, use a single asterisk to replace the number (*.cas.h5). Reader supports reading Fluent mesh files (.msh.h5), instead providing (.cas.h5) select only (.msh.h5) file and click on Load all parts
Format Options Tab
Fluent HDF5 reader options
Load Internal Parts	Toggle this ON to load the Fluent Internal/Interior Parts. This will show all the internal walls forming all the cell volumes. If you do toggle this on, then you should click the Choose Parts button at the bottom of the data reader dialog, rather than Load all, as you'll only want to load the interior parts of interest to save memory and time. Default is OFF
Load _M1 _M2 vars	Variables that end in _M1 and _M2 occur in Fluent unsteady flow. They represent the value of the variable at the prior iteration time and the time prior to that respectively. By default this toggle is OFF and these variables are not loaded. Toggle this ON to load these variables.
Load all cell types	Fluent cells have a boundary condition flag. By default (toggle OFF) EnSight loads only the cells with a boundary condition flag equal to 1 (one). Toggle this option ON to load all cells with a non-zero boundary condition. For example, if you have a part with cells of boundary condition 32 (inactive), EnSight will, by default not load this part. Toggle this option ON and EnSight will load this part. Note:  Parts containing cells with a boundary condition of zero are never loaded.
Poly to Regular Cell	Fluent polyhedral cells when composed of the correct kind and number of regular faces can be converted to regular cells (tetrahedrons, hexahedrons, pyramids, or wedges) boosting EnSight speed and decreasing memory requirements. Toggle ON and reader checks each polyhedron to see if it can be converted to a regular cell (default) and OFF to not convert any polyhedral cells. There is very little slowdown during the read to do this and a big payoff for some datasets with large numbers of convertible polyhedra. Leave it on.
Poly faced Hex to Poly	Fluent hex cells that transition to a more refined hex mesh will sometimes have one or more of the quad4 faces subdivided into four quad4 faces. For example, a hexahedral cell with one transition face will have the six full faces, and four subdivided faces for a total of 10 faces. Toggle ON and the subdivided faces are kept rather than the full face and the cell is changed into a polyhedral which will slow down EnSight performance, and greatly increase memory. The polyhedral also will have hanging nodes (see the next toggle). Toggle OFF (default) to convert the hex element to a six-sided hex which will be adjacent to four smaller cells rather than completely connected to them slowing down EnSight's adjacency searching. The default is thought to be the lesser of two evils.
Fix Hanging Nodes	Some Fluent polyhedral cells and all transition hex cells converted to polyhedrals will have hanging nodes. A hanging node is a node not shared by at least 3 faces. A polyhedral element with hanging nodes is not watertight and can cause real problems in EnSight, so it is best to leave this toggle ON (default) and only turn it OFF for experimental purposes.
Use Zone IDs for Parts	A heterogeneous mix of serial and parallel solution files will result in a jumbled part ordering between cas.h5 files. Toggle this ON to use the part zone id to reorder the parts consistently from .cas.h5 file to .cas.h5 file using the first file loaded as the canonical order.
Show Fluent Variable Display Name	When this toggle is OFF legacy variable names are used, and when ON (default), the restart reader will match the Fluent variable ID from a variable map file ANSYS_FLUENT.xml (included in the EnSight install) which will allow EnSight to use the Fluent graphical user interface variable name. EnSight will use the variable map file to determine which variables to make available to the user.
Enable Part Grouping	This option allows the reader to group the Fluent cell zone and adjacent face zones. Default it is turned OFF. Unless both .cas.h5 and .dat.h5 are provided this option won’t work.
Console Output	Use this flag to determine the amount of output to the console. Normal - Usually only echo errors to console. Verbose - Normal output plus an echo of every Fluent part that is in the dataset, whether it is interior or not, whether it is skipped, what variables are defined for which parts, and to echo it's EnSight Part number. Debug - Verbose output plus more detailed output and progress through the reader routines often valuable for understanding and reporting problems.
Time Values	Use Filename Numbers will read the sequential numbers at the tail of the filenames and adjust them by making the first number 0 and shift all subsequent values adhering to following situations. If number of cas.h5 files equal to number of dat.h5 files file4000001.cas.h5, file4000004 ... file4000020 timestep 0 has time value 0.0, timestep 1 has time value 3.0, and timestep n has time value 19.0. If there is a single cas.h5 file and multiple dat.h5 files it defaults to Use Time Steps Use Time Steps will make timestep and time value the same for example: timestep 0 will have time value 0.0 and timestep 5 have time value 5.0. Read Time Values (default) will open each file and find the exact time value using the 'flow-time' keyword. This means that every file has to be opened and searched. It’s possible that user may supply single cas.h5 file and multiple dat.h5 files which are written during steady analysis. In that case reader defaults to Use Time Steps Calc Const Delta reads a delta time from one file using 'physical-time-step' keyword, and calculates the time values by multiplying the delta value by the adjusted filename number. It is essential that your time values are correct for some calculations (for example, if you are going to do pathline tracing). Consider that if your timesteps are uniform then you can use the Use Time Steps option and just scale your time values using the Time Options tab in the data reader dialog. If your timesteps are not uniform, but your File Numbers are proportional to your timesteps then you can select Use Filename Numbers and then scale the time values using the Time options tab in the data reader dialog.
Project File Name	Provide the name of the Fluent Project file (.flprj) written out by Fluent during the save of the .cas.h5/.dat.h5 (default empty). This project file, which is written by the solver, contains meta data regarding time value and .cas/.dat pairs. The specification of this filename, while optional, is encouraged when working with transient data to more robustly handle time values and .cas/.dat pairings. If no path is given (filename only), the routine will search the directory given by the .cas/.dat specification for this file. If no file is given, the reader will search the directory given in the .cas/.dat file specification. If a single file is found, the reader will attempt to use it. If multiple files are found (but none specified), the reader will not know which one to utilize and will therefore proceed with no project file.

Node and Elem IDs

Parts have node and element ids to enable querying your data. Node ids are created from the coordinate global node. Element ids are created as follows. Face part elements are uniquely numbered according to their zone index. Cell part elements are uniquely numbered using their zone index added to the total number of faces. So a dataset with 100 face elements and 300 cell elements would have the face elements number 1-100 and the cell elements numbered 101-400. In Verbose mode, the element id range for each part are written to the console.

Part Order and Name

Part name and its order (sequence) appearing in EnSight’s part list is provided by CFF SDK. While reading transient dataset, the reader tries to maintain a global part list i.e. it scans all cas.h5 files and try to find out if number of parts are changing over time and creates a single part list which remains present at all the time-steps.

Variable Location and Name

Fluent dat.h5 restart file has cell-centered solver specific variables’ data and this reader does not interpolate the cell-centered variables to the nodes. The reader attempts to identify the Fluent display variable name based on each variable’s sub section id provided by CFF SDK. If it’s not found reader may skip such variables with appropriate warnings.

Variables Undefined

Not all variables exists on all parts in .dat.h5 file. If you select a part and color by a variable and it is undefined; it means that selected variable is not defined for selected part and EnSight does not have the boundary conditions nor the solver physics algorithms to extrapolate variable values to boundary parts. Create a clip on the location of an interior part on a volume part if you want to see a plane with values from the volume.

Extra Variables

EnSight will try to calculate extra CFD variables given existing dat.h5 variables for your convenience.

CAS.H5 Constants

Extra single Value Variables - A number of single value variables are read from the .cas.h5 file(s). These will show up in the EnSight Calculator named as follows.

PRESSURE_ABS - operating pressure (absolute)

PRESSURE_ABS_INIT - initial operating pressure (absolute)

GAMMA_REF - reference gamma, ratio of specific heats

VISCOSITY_REF - reference viscosity

TEMPERATURE_REF - reference temperature

PRESSURE_REF - reference pressure

DENSITY_REF - reference density

SPEED_SOUND_FAR - far field speed of sound

PRESSURE_FAR - far field relative pressure

DENSITY_FAR - far field density

R_ref - Calculated reference gas constant = (PRESSURE_ABS / (DENSITY_REF * TEMPERATURE_REF)

V_def - Calculated default velocity magnitude from x, y and z- velocity default values M_def - Calculated from V_def / SPEED_SOUND_FAR

Polyhedral Elements

This reader will attempt to convert polyhedral elements back to regular elements, saving memory and speeding up EnSight.

Particles

Currently, the Fluent HDF5 reader handles Discrete Particle data and variables for those particles which are explicitly saved into the .cas.h5 and/or .dat.h5 files. The reader does NOT read in particles stored in other files (PDF files), nor particle information which is generated within Fluent Post interactively. For models which are running steady state continuous domain, you can have either steady particles, or unsteady particles computation. Only those situations where the particle data is explicitly written to the .dat.h5 or .cas.h5 files can be read by this Fluent HDF5 reader. It may appear like you see discrete particles in Fluent, but if they have not been explicitly written to the .dat.h5 or .cas.h5 file, the Fluent HDF5 reader will not be able to read them/provide them to EnSight. For models which are running transient continuous domain, the Fluent HDF5 reader will only be reading particle data from the .dat.h5 file, which may be coarser (temporally) than typically desired. We will attempt to address this shortcoming in the future Ansys Fluids Post format.

Variable Naming

The variables show in the variable list are determined by an internal, Ansys API. Therefore, the variables shown in this reader may differ from those shown in the Fluent cas/dat reader (which reads and shows all the variables directly from the .dat file).  Further the variable names are also determined by the Ansys API and therefore may be different from the Fluent cas/dat reader, which names variables to traditional, reasonable, legacy text names.

Limitations

The Forte reader is supplied with EnSight to read .ftind index file that is output from the Ansys Forte solver. Select the .ftind file to use the EnSight Forte to read your geometry and variable solution data into EnSight.

The LS-DYNA reader reads in a single or multiple unstructured C-binary d3plot files.

It supports bars, quads, bricks and thick shell elements.

Key File for Part Naming

Can use of Key file to name parts as follows:

FEMZIP

The reader uses the publicly-available femunzip utility to unzip the compressed files. This unzip utility can be downloaded for free. The user must set the environmental variable FEMUNZIP_UTILITY_PATH to point to the location of this executable. The reader will call this executable on the d3plot file(s) to ensure that the file(s) are unzipped into a temporary folder prior to reading. A mapfile.txt pointing to the unzipped files will be created which will be used in subsequent runs avoid the need to unzip again.

CFD Data

The reader skips legacy CFDDATA sections, and reads instead the ICFD data from the incompressible CFD and incompressible CFD surface solvers.

DEM/DES

The reader now includes this particle data.

AMR

The reader can read AMR data even if the expected, first d3plotaa is not available.

Duplicate Timesteps

The reader skips duplicate timesteps, caused perhaps by double precision to float conversion.

Limitations

The reader has the following limitations:

See the following file for current information on this reader.

After the notation regarding $CEI_HOME/ensight251/src/readers/ls-dyna3d204/README.txt, users utilizing ALE Solutions will see additional variables listed as el8_var01, el8_var02, etc. These variables correspond to material volume fractions for the various of materials specified in the ALE solution.

In addition, pressure is stored in the stress field variables and can be displayed by computing a new variable in EnSight's calculator equivalent to the negative of the average of the three normal stresses:

Simple Interface Data Load

Load your d3plot file using the Simple Interface method.

Advanced Interface Data Load

Load your d3plot file using the Advanced Interface method.

Data Tab
Format	Use the LS-DYNA3D format.
Set d3plot	This field should have the first d3plot file name. All of the d3plot files will be loaded starting with this first one
Set key	This field can be used to import parameters that modify the behavior of the reader, or the Extra GUI section can be used to choose which ids to use for naming and to name the keyfile respectively. keyfilename - Type the keyfile name into this field -mid - use material id in keyfile to name parts in d3plot file. -pid - use part id in keyfile to name parts in d3plot file. Example 2.9: Mid/Pid file.key -mid This will use the material ids in keyfile named file.key to name parts.
Format Options Tab
Set measured	Select the measured file and click this button.
Format Options	The following options are customized for the reader:
Remove Failed Elems	Failed elements will not be shown (default)
Use ALE Variables	Include the ALE variables
Keyfile IDs	This pulldown provides the choice of either Material IDs or Part IDs from the keyfile to be used for part naming.
d3plot IDs	Use either Material IDs (default) or Part IDs within the d3plot file to read in the data.
Console Output	Can control amount of output that comes to the console. Options are: Normal, Verbose, or Debug
ASCII File Input	Can input glstat, abstat, matsum, rcforc, rwforc, nodout, secforc, sleout, elout, dbfsi, and spcforc xy ascii files as EnSight xy queries. These files must be in the same directory as the d3plot file(s). Choose none (default) or all for all of the available files. Choose filenames.txt if you wish to name a subset of the files to read.
Binary (binout) File Input	Can input the binout file (default none) glstat, abstat, matsum, rcforc, rwforc, nodout, secforc, sleout, elout, dbfsi, and spcforc and nodfor, or all curve sets as EnSight xy queries. The binout file must be in the same directory as the d3plot file. This uses the LSTC binout API to read the xy data.

See Read Data

The LSTC-LS-DYNA Reader is a completely new, optimized implementation that uses an API written by LSTC (the authors of LS-DYNA) to read in a single, or a series of C-binary, d3* files (built on the d3plot framework), exported from the LS-DYNA solutions for post processing. Since the reader is built upon an API designed by the authors of the solver it should be expected to read the most current format updates (included FEMZIPPED data), and the broadest support for the families of solutions within the LS-DYNA application. The new reader is faster and provides a better LS-DYNA user experience than the legacy LS-DYNA Reader reader (which is still available, but not the preferred reader option).

Requirements

This reader uses version 0.1.41 of the LSTC API, which is included with your EnSight installation on Windows and Linux (Apple is not supported by the API). This supports d3* post processing files exported from version R12, and earlier versions of the LS-DYNA solver.

User Information

User messages from this reader (informational, warnings and errors) appear in the Message Box Overview. If problems are encountered, the user can choose Console Output Debug in the Format Options tab in the Data Reader dialog with the LSTC reader chosen and the advanced toggle on. This will put a voluminous amount of debug output in the message box which can be saved and sent to Ansys support.

Supported Solution Types

- ACC - Ansys Acoustic method solver file d3acc

- ACP - Ansys Composite PrePost solver file d3acp

- ACS - Car Cabin Acousics (ACS) solver file d3acs

- ATV - Acoustic Transfer Vector solver file d3atv

- EIGV - Eigenvalue/vector modal analysis file d3eigv

- ERP - Equivalent Radiated Power solver file d3erp

- FTG - Fatigue solver file d3ftg

- DRLF - Dynamic Relaxation Phase file d3drlf

- PSD - Power Spectral Density file d3psd

- RMS - Root Mean Squared file d3rms

- SSD - Steady-State Dynamics file d3ssd

Units

Neither LS-DYNA nor the exported post processing files support units. It is entirely the responsibility of the analyst to choose self-consistent inputs prior to running the analysis.

BINOUT XY Query Data

LS-DYNA saves xy queries in a standardized binary format in branches; each branch represents a category of xy data that was formerly an individual ascii file. Within a branch, a query might be a variable value over time, at a given location (nodal or elemental), within a set of grouped queries. A branch with a number of sets, a number of variables and a large number of node or element ids, can contain a very large number of XY query permutations. Also, these xy queries can have high sample rate time history data, resulting in a very large number of xy pairs.

Unfortunately, EnSight’s initial design of the query interface had in mind a relatively small number of queries with a relatively low sample rate. So, EnSight is currently very inefficient at the initial load of large number of queries especially those with a high sample rate. Currently EnSight reads in all of the xy data at the initial load and sends the xy pairs all up to the client, and has no mechanism to ‘activate’ queries, thus greatly increasing the initial load overhead), and then, after the load has no mechanism to organize and present and manage large numbers of queries (it lacks the ability to group and subgroup and tag queries in the query interface). So the limited implementation of binout data are currently considered for demonstration purposes only.

Currently the reader has limited support for two branches within the binary, binout datafile: spcforc, and nodfor time history data. When the binout file is entered into the second field in the data reader dialog, then the Message window will contain output indicating what branches are available and which ones are loaded. When nodal query data is available and supported, Query Parts (point parts) are created to spatially show nodal query locations in the graphics area and to allow users to right click on a query location node, and choose to plot the available queries at the selected location. However, given the current EnSight query interface limitations, the number of node or element ids is currently limited to 100 in order to keep the number of queries manageable. Support for time history branches will be added over time in this reader and the handling of large query data branches is expected to improve within EnSight as well in subsequent versions.

Sample Message Box Output

XY Query groups available in the BINOUT file

1. 'glstat'

Warn WARNING: Found 'glstat' xy data, but not implemented yet

2. 'matsum'

Warn WARNING: Found 'matsum' xy data, but not implemented yet

3. 'rcforc'

Warn WARNING: Found 'rcforc' xy data, but not implemented yet

4. 'spcforc'

number of XY Queries = 603

Parts and Materials

The reader supports the regular element types: spherical particles (as 0D point elements), bars (as 1D line elements), quads (as 2D surface quadrilaterals), bricks and thick shells (each as 8 node hexahedrals). Parts are formed out of element using material ids. Currently the actual material associated with the material id is unavailable in the post processing files and the LSTC API does not read the LS-DYNA input analysis key file (*.k or *.key) file where this information is found. Regular parts will be of KIND Regular. Part names will include the material ID as well as the part name, if it is available. For legacy datasets, where the part name is unavailable then only the material ID will be used as the regular part name.

Parts containing only points will also be formed for some branches of binout data to indicate the query location. These binout parts will be located in a Part group named XY_Query_Location, and each Query Part will named according to one of the branches: nodfor and spcforc and will have a point field, with each point representing a query location, and each point node id representing the query node id. A Query Part KIND is XY query locationnid. Initial query part visibility will be off, and the points will be represented initially as a cross and colored purple when the part is made visible to show the query locations. See Advanced for how to use the Query Parts.

When MS data is loaded, Parts that are Regular will be put within the Structural group (named using their material id and their part name, and they will have KIND Regular). MS parts will be grouped by their MS domain. Each MS part will be of KIND MS_Shell, MS_Solid, or MS_Beam to indicate their origin and their element type.

Transient

For transient data, Parts are either changing coordinates only (connectivity and nodes stay the same through time and only the xyz values of the nodal coordinates update through time) or changing connectivity (Nodes, xyz location, as well as the elements’ connectivity all change through time; this is called an adaptive mesh in LS-DYNA). This is an EnSight global, so if any part is changing connectivity, then all are changing connectivity.

If the data is a frequency analysis, then timesteps and time values become modes and frequency values. A case constant variable named Frequency is available as the actual frequency value.

Variables

This reader creates single-value constants (transient single value per timestep), per part constant (transient single value per part), scalars, vectors, and plug-in (Python calculated) variables.

Variables are presented in the way that is most useful within EnSight (for example, Tensor variables are presented as Scalar components of the Tensor, such as Stress_XX) and named in a way that is most useful within EnSight (for example, noun_adjective_adverb): Strain_Effective_Plastic. Where variables are named within the Solution family (such as Multi-Solver, MS solution data) the variable name in the file is used (sans the forbidden characters Variable Creation). Variable values can be written in the database for certain parts in certain domains or for certain element types and not for others; the reader will handle this by defining the values where they are available and telling EnSight that the variable is undefined where it is unavailable.

Some variables are needed by you but are unavailable in the post processing files. They are made available as EnSight Python Plug in variables and include the following: Stress_Principal_Min, Stress_Principal_Min, Stress_Principal_Min, Stress_Tresca, Stress_Von_Mises, which will show up if the required six stress component scalars are available (Stress_XX, Stress_YY, etc. ). If these are activated, then the required six stress component scalars will also be activated, and an EnSight Python plug in will perform the required calculation to create these variables.

Multi-solver variables are available on MS part nodes or elements. Some Electro-Magnetic variables may not have the correct name (appearing as Var_01, Var_02, etc.) but their values appear correct relative to LS-PREPOST. The Centroid variable is currently undefined on multi-solver elements. A workaround would be to use the EleMetric calculator function and select Centroid from the Predefined function parameters.

A single value is available for each scalar or vector component on each element. However that element may contain a number of values at each of the element integration points (IPs). You have the option at the time of the data read to choose one integration point location for the shell elements (inner, mid, or outer), or to combine them (min, max, or average of the three locations), or to combine all of them (if there are more than three, min, max or average of all the integration points. For the other elements, the user has the option of of min, max or average of all the integration points. The default for all element types is to present the max of all the integration point as the single value at that element. There is no option to change this choice except to reload the data and pick another option.

LS-DYNA conditional variables are supported (a single variable location within the d3plot that is used to store values for completely different variables depending on the analysis type). This includes History variables. Which variable will remain unknown to the reader, because naming them requires the ability to parse the input (*.k, *.key) file, to figure out the analysis type and to use a lookup table to find the name. These variables appear in EnSight, for example, with cryptic names, such as Shell_Var01, Shell_Var02, etc where these particular variables can represent the following, depending on the analysis and/or material type, which should be known to the user.

Apparent Variable Discontinuities Across Part Boundaries With ALE Solutions

LSPrePost interpolates variables globally (across parts), while EnSight interpolates variables part by part. In the ALE solutions of LS-Dyna, the elemental-stored values can have discontinuities from element to element, which can result in variable coloration which illustrate this discontinuity between parts in the data. If this rendering discontinuity is undesirable, there is method to handling discontinuities across parts by issuing the command test: across averaging on in EnSight’s Command dialog. Once turned on, you can then create a new variable by using the ElemToNode() calculator function to interpolate the elemental variable to the nodes (using averaging across parts) to generate a smoother nodal variable field.

Simple Interface Data Load

Load your LS-DYNA file (typically named d3plot or file.d3plot, or any variation such as d3acc, etc.) using the Simple Interface (Simple Interface) method.

Advanced Interface Data Load

Load your LS-DYNA file (d3plot or file.d3plot, or any variation such as d3acc, etc.) using the Advanced Interface method.

Data Tab
Format	Use the LSTC-LS-DYNA format.
d3file	Choose one of the following that have been tested: d3plot, d3acs, d3acp, d3atv, d3eigv, d3erp, d3ftg, d3psd, d3rms, d3ssd, d3thdt, d3zcf, drlf , or choose other similar d3* or d* post processing file and click on the d3file button.
Binout	Choose a binout file and click on the binout button.
Format Options Tab
Use Part Metadata	(default ON). Sets part KIND, MATERIAL (when this becomes available from the input (key) file, grouping, default coloration, point display type (if point part). This will create Query Parts if the binout file is selected in the second field and it contains a supported nodal query branch. This will also auto generate regular part groups, using the first three digits of the part id, if the part ids are greater than 100,000 and the if number of parts is greater than 200.
Console Output	Normal, Verbose, or Debug, default is currently Verbose. Errors and warnings are always printed out. Normal is typically minimal informational output, Verbose is output considered of interest to the curious user, and Debug output is designed as a window into the data itself, particularly useful for detailed, reporting of problems to Ansys support.
Shell IP option	Mid, Inner, or Outer – A single IP of one of these three. Max, Min, or Avg of the above three. Max, Min, or Avg of all (if there are more than three). Default is Max All.
Non-Shell IP option	Max, Min, or Avg of all. Default is Max All.

Advanced

LS-Dyna sometimes writes out non monotonically increasing time values. EnSight does not support this type of data. The reader will attempt to tweak duplicate time values with a small delta time, and if that is not successful, then will make timesteps integers, starting at 0.0 and incremented by 1.0. Or, frequencies, which appear as separate timesteps will sometimes not be increasing with timestep. In this case, the reader will make a constant variable named Frequency, and will make the timesteps integers starting at 0.0 and incremented by 1.0.

The reader will send a flag up to EnSight for deleted elements, Filter Part Elements, Filter Parts.

If you have loaded binout data and you have xy query parts loaded, you can use these points to pick the location where you would like to see a query plotted. Make the query part visible that represents the binout branch of interest in order to see the points in the graphics area, then turn on node ids, and right click on the point of interest (see below, and notice the top of the right click menu says Part 3 nodfor, confirming that you’ve right clicked on a point in a query point part, in this example, node id 11501), then choose Plot model query… and see the pop up window so choose from all the queries that are available for node id 11501 as shown below. Click OK to see a plot of the selected queries in a single plot.

Limitations

The following are currently unsupported:

Reads any of the following (in preferred order):

See the following file for current information on this reader.

$CEI/ensight251/src/readers/dytran/README.txt

Simple Interface Data Load

Load your dytran file (typically named with a suffix .dat or .arc) using the Simple Interface method.

Advanced Interface Data Load

Load your dytran file (typically named with a suffix .dat or .arc) using the Advanced Interface method.

Data Tab
Format	Use the MSC/Dytran format.
Set dytran	The preferred input is the file with .dat suffix. The root name of this file will be used to find all .arc files in the directory which match the Dytran naming convention. And all parts of the model will be made available to EnSight. Additionally, this method allows for the most efficient setting for changing geometry, because it can glean some pertinent information thereto within the .dat file. Alternatively, you can enter one of the .arc files, and all .arc files in the directory which match the pattern will be found and used. Note:  No widcards are needed - just select one of the .arc filenames. The third method is to enter a custom case file. This user generated ASCII file allows one to specify particular parts, etc. Since one can accomplish the same thing by only loading specific parts within EnSight, this method is probably obsolete.
Format Options Tab
Set measured	Select the measured file and click this button.
Format Options	The following options are customized for the reader, in version 2.05 or later.
	Make vector vars from standard scalars - Toggle on to have vector variables automatically generated from known standard scalar components. On is the default. Example: If toggled on, a vector variable named VEL will be created from the scalars XVEL, YVEL, ZVEL
	Load Time History Queries - Toggle on to have all xy time-history queries (contained in pattern matching .THS files in the directory) loaded automatically into EnSight. On is the default. Note:  These have traditionally been read into EnSight in the Query/Plot feature, but reading each .ths file as an external file. While this option still exists, it is not needed if this toggle is on.

If you choose to not have the Dytran XY time-history data (from the .ths files) loaded automatically, or if you are using a prior version of the reader, you can later click on the XY Query/Plot icon and choose to load data from an external file in the pulldown, and choose the desired .ths file(s). For details, see Queries From External Sources.

See Read Data.

Reads a t16 or t19 file (which is the preferred method).

See the following file for current information on this reader.

Simple Interface Data Load

Load your marc file (typically named with a suffix .t16 or .t19) using the Simple Interface method.

Advanced Interface Data Load

Load your marc file (typically named with a suffix .t16 or .t19) using the Advanced Interface method.

Data Tab
Format	Use the MSC.Marc format.
Set t16/t19	This field should have the .t16 or .t19 suffix file.
Format Options Tab
Format Options
Include ElemSet Parts	Include any Element sets defined. These are sets of full elements which are generally some logical subset of the total number of elements. Default is on.
Include Face/Edge Set Parts	Include any Face or Edge sets defined. These are some logical set of particular faces and/or edges of full elements. Default is on.
Include NodeSet Parts	Include any Node sets defined. These are generally the subset of nodes needed for the Element, Face, or Edge sets above. As such, they are generally not needed as separate parts, but can be created if desired. Default is off.
Include local elem res comps (if any)	Include the local stresses components, etc that are in the element's local system. A simple example is a bar (such as a truss element), which only has tension or compression in the element's axial orientation. Such an element would have an axial stress variable. Other elements would have appropriate result component variables. Default is on
Include Tensor derived (VonMises, etc.)	For tensor results, calculate scalars from the following derived results (principal stress/strains, and common failure theories): Mean Equal Direct VonMises Min Principal Octahedral Mid Principal Intensity Max Principal Max Shear By default, all 9 of these will be derived. You can control which are created by this toggle, with an environment variable. Namely, setenv ENSIGHT_VKI_DERIVED_FROM_TENSOR_FLAG n where n = 1 for Mean only 2 for VonMises only 4 for Octahedral only 8 for Intensity only 16 for Max Shear only 32 for Equal Direct only 64 for Min Principal only 128 for Mid Principal only 256 for Max Principal only 512 for all or any legal combination. example: for VonMises and Max Shear only, use 18. Default is on.
Regular Part Creation Convention	Parts will be created according to the following:

See Read Data

There are two Nastran readers: Nastran OP2, and Nastran OP2 (beta). Both read .op2 files, and the beta version additionally reads XDB files. This section documents only the Nastran OP2. It reads .op2 suffix files including most PDA Patran (PARAM POST = -1) and SDRC I-DEAS (PARAM POST = -2) files.

Limitations

Recent Enhancements

README

See the following file for current information on this reader.

$CEI/ensight251/src/readers/nastran/README.txt

Simple Interface Data Load

Load your geometry/results file (typically named with a suffix .op2) using the Simple Interface method.

Advanced Interface Data Load

Load your geometry/results file (typically named with a suffix .op2) using the Advanced Interface method.

Data Tab
Format	Use the Nastran OP2 format.
Set op2	Enter the .op2 filename if reading a single NASTRAN .op2 file, or a .mop filename if reading multiple .op2 files. The .mop file is an ASCII file listing .op2 filenames. See the description above or the README file indicated above for more details.
Format Options Tab
Set measured	Select the measured file and click this button.
Extra GUI	The following parameters are available. They are described below.

Format Options Parameters

The toggles and fields below are customized for the Nastran OP2 reader. They allow the user to specify basic options before the data is read. They may not all apply to any given model.

Include 1D Elements

Toggle on to include any 1D (bar, rod, etc.) elements.

Include 2D Elements

Toggle on to include any 2D (tri, quad, etc.) elements.

Include 3D Elements

Toggle on to include any 3D (tet, hex, etc.) elements.

Rigid Body Timeline Controls

Toggle on to have the geometry timeline controlled by the rigid body times (if present). If off, the flex body times in the .op2 file will control.

Convert Modal Freq to Time

Toggle on to compute solution time from the frequency field in the file for eigen analysis (default is on). The is done with . Toggle off to no perform this computation and instead read the frequency value as the time.

Elem Var

This pulldown provides control over the way Nastran element values will be presented as variables within EnSight.

Elem Var Type

This pulldown provides the choice of extracting either Strain or Stress from Nastran element values.

GridPt Var Type

This pulldown provides the choice of extracting either Strain or Stress from Nastran Grid Point values.

1D Bar Loc

This pulldown provides the choice of where along the bar (EndA, EndB) or across the cross-section (Pts 1-4), and what type of stress or strain to extract from Nastran bar elements.

2D Shell Fibre

This pulldown provides the choice of which cross-sectional fibre (@Z1 or @Z2) to extract from Nastran 2D Shell elements.

GridPt Surface Loc

This pulldown provides the choice of which cross-sectional fibre (@Z1, @Z2, or @MID) to extract from Nastran 2D Grid Point surfaces.

Part Creation

This pulldown provides part creation choices (which are most useful when a .mop file is used to bring in multiple OP2 files together:

NX Nastran Version:

This pulldown provides you with some control over the changes that occurred in the element record length at NX Nastran version 4.0. This is needed because there is not a good way to determine the version used from the .op2 file itself.

2D Composite ply:

This field allows the user to specify from which ply number to extract values from Nastran 2D composite elements

See Read Data.

Description

Reads OpenFOAM controlDict file found in modelname/system/controlDict.

File → Open...

The File Selection dialog is used to specify which file you wish to read.

File → Open...

Handles steady state geometry with either steady state or transient variables. Steady state variables with multiple iterations will use each iteration as an EnSight timestep.

Not yet supported :

Ongoing solution. The reader cannot handle newly available timesteps or iterations (for example from an ongoing OpenFOAM solution) after the model has been read into EnSight the first time. Should new iteration or timesteps become available after the model was originally read into EnSight, the user must reload the dataset.

Command Line Data Load

To automatically start EnSight and load the current directory's OpenFOAM dataset from the command line, type ensight -Eensfoam. This will trigger EnSight to start up, look for the current directory's system/controlDict file, and automatically load the dataset into EnSight (using the default reader settings). This reduces the number of steps to load the file into EnSight and therefore the real time required to load the data, and provides a level of integration with this data format.

Sample Data

A sample OpenFOAM dataset is included as a sample session with your install. To access the welcome screen, at the top menu choose Window → Welcome To... and load the Dam Break example session. Or, to load the same dataset manually, find the controlDict file in $CEI/ensight/other_data/openfoam.

Simple Interface Data Load

Load your OpenFOAM controlDict file using the Simple Interface method. Or from the command line, simply run ensfoam.

Advanced Interface Data Load

Load your OpenFOAM file using the Advanced Interface method.

Data Tab
Format	Use the OpenFOAM format.
Set file	This field contains the controlDict file. Clicking this button inserts the file name shown into the field.
Format Options Tab
Set measured	Select the measured file and click this button.
Other Options
Include ElemSet Parts	Include any Element sets defined. These are sets of full elements which are generally some logical subset of the total number of elements. Default is on.
Generate Wall Parts	Generate 2D Face Sets. Default is on.
Include between processor surfaces	If toggled ON and the data is from a parallel solution, then the surfaces between the processors will be generated as parts. Default is off.
Check and cap infinite results	If toggled ON and there exists values in the file that are beyond the 32-bit size limit (therefore creating 'inf' infinite values), they will be capped at a value just below that limit value. Default is off
Regular Part Creation Convention	Parts will be created according to the following: Use Part Id - Part Id (this is the default) Use Property Id - Property Id Use Material Id - Material Id
Var naming convention	Use DataSource field - By default variables are named using the variable filename. For example, "U" is velocity, "p" is pressure, etc. Use Content Field (if provided) - Known variables are given full, meaningful names, for example, "Velocity" or "Pressure". Use VKI dataset name - Long, hybrid variable name including the VKI variable dataset name.
Particle Part Separation	Parts will be separated according to the following: None - Remains within the original part Separate parts if particles in 1st step - Creates separate parts without particles (default) Separate for ALL parts (can be empty) - Creates separate parts for ALL original parts (even when empty)
Element Vars as	Single element values - Element results (whether centroidal or element nodal) will be presented as a single value per element. Therefore will be per_elem variables in EnSight. This is the default. Averaged to node values - Element results (whether centroidal or element nodal) will be averaged to the nodes without using geometry weighting. Therefore will be per_node variables in EnSight. This is a global averaging, so shared nodes are affected by all parts that share a node. Geom weighted average to node values - Element results (whether centroidal or element nodal) will be averaged to the nodes using geometry weighting. Therefore will be per_node variables in EnSight. This is a global averaging, so shared nodes are affected by all parts that share a node. Ave to node values <by parts> - Element results (whether centroidal or element nodal) will be averaged to the nodes without using geometry weighting. Therefore will be per_node variables in EnSight. This is a local averaging, so all averaging is contained within each part. Geom weighted ave to node <by parts> - Element results (whether centroidal or element nodal) will be averaged to the nodes using geometry weighting. Therefore will be per_node variables in EnSight. This is a local averaging, so all averaging is contained within each part.

See Read Data.